Training Guide Basics

Transcription

1 Training Guide Basics

2 2014, Missler Software. 7, Rue du Bois Sauvage F Evry, FRANCE Web: All rights reserved. TopSolid Design Basics This information is subject to change without warning. No material may be reproduced or transmitted, regardless of the manner, electronic or mechanical means used or purpose, without formal written consent from Missler Software. TopSolid is a registered trademark of Missler Software. TopSolid is a product name of Missler Software. The information and the software contained within this document are subject to change without prior warning and should not be construed as a commitment by Missler Software. The software covered by this document is supplied under license, and may only be used and duplicated in compliance with the terms of this license. Version 7.8 Rev.01 Note: If you are experiencing problems using this training guide, please feel free to send your feedback and comments at edition@topsolid.com. ii Missler Software

3 TopSolid Design Basics Contents Exercise 1: The axis sketch... 1 Creating a new project... 1 Creating a new part document... 2 Creating a sketch by points... 2 Modifying the sketch... 4 Exercise 2: The second sketch... 6 Creating a new part document... 6 Creating the sketch... 6 Exercise 3: The bracket Creating a new part document Creating a sketch by points Creating the part Drafting the part Creating a new sketch in the part document Assigning properties Exercise 4: The clamp Exercise 5: The handle Creating a new part document Creating the first sketch Creating the second sketch Creating the revolved surface Creating the extruded shape up to the surface Creating the third sketch Creating the boss Creating the tapped hole Declaring the part representation Assigning properties Drafting the handle Exercise 6: The flange Creating a new part document Creating the sketch Creating the shape Creating operations on the shape Modifying the pocket sketch Missler Software iii

4 TopSolid Design Basics Assigning properties Modifying one of the drillings Exercise 7: The key Creating a new part document Creating the sketch Creating the shape Assigning properties Exercise 8: The roller Creating a new part document Creating the sketch Creating the shape Assigning properties Exercise 9: The roller draft Creating the draft document Creating the main view and auxiliary views Modifying the part The roller Updating the draft and adding detail views Exercise 10: The cam Exercise 11: The axis Creating a new part document Creating the sketch Assigning properties Exercise 12: The elbow Creating a new part document Creating the sketch Assigning properties Exercise 13: The puncher Creating the body Creating the assembly document Creating the in-place sole Importing a Parasolid file Retrieving the publishing Positioning the handle Searching the libraries for a spring Creating screws with their repeated drillings iv Missler Software

5 TopSolid Design Basics Exercise 14: The PDM Project organization Importing a package in the PDM folder Document structure Using the file backup and its options Data security Modifying a part Data security Document history Purging minor revisions Life cycle References Back references Modifying the plate Checking the references of the puncher Redirecting the last major revision of the plate on the puncher Making obsolete the A revision of the plate and the puncher Modifying the handle B.0 major revision Copying and pasting the Puncher document Redirecting the back references of the Handle document Redirecting the references of the Puncher 2 document Deleting the Puncher 2 document Deleting the B revision of the handle Using the PDM in Client/Server mode Exercise 15: Creating document templates Creating a new project template Declaring the new project template Creating a new part template Declaring the new part template Creating a new draft template Notes Individual Course Evaluation Form Missler Software v

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7 TopSolid Design Basics Exercise 1: The axis sketch Exercise 1: The axis sketch Concepts addressed: - Creating a new project - Creating a new part - Creating a sketch by points - Editing and modifying a sketch - Saving work Creating a new project From the Home tab, create a new project by clicking on the icon. In the Name field, rename your project as follows: Your name Basics Training. In the Template field, select Blank Template and confirm by clicking on the green check mark. Once validated, the following new project is created and automatically appears in the Project tree. Missler Software 1

8 Exercise 1: The axis sketch TopSolid Design Basics Creating a new part document In the Project tree, right-click on the project name and select the Document function. In the Type section, click on the Common tab and select Part as the type of document. In the Template section, select Blank Template and click on to confirm the creation of the document. The newly created part document automatically opens. In the Project tree, rename this part The axis sketch and validate by pressing the Enter key. Creating a sketch by points In the 2D Sketch tab, create a contour by points by clicking at the frame s origin, then stringing together the remaining points. To close the contour, click either on the first created segment (AB), or on the last created segment (EF). Confirm the creation of the contour. This produces the result shown opposite. 2 Missler Software

9 TopSolid Design Basics Exercise 1: The axis sketch Note: The contour is made up of segments with two different colors: - Blue for fully constrained geometries. - Magenta for underconstrained geometries. Using the Constraint icon, dimensionally constrain the BC and DE segments as seen opposite. Similarly, constrain the angle formed by the DE and EF segments. Note: As it is the contour of a cylindrical part, the next two dimensions will be revolution dimensions. The default revolution axis is the X axis. If you want to change it, use the 2D Sketch > Define Revolution Axis command. Select the Revolution Dimension function and dimension the BC segment, and then point D so as to obtain the result shown opposite. Adjust the contour by modifying the dimension values in order to produce the result seen below. To do this, double-click on the dimension to be modified, enter the new value and click on. Repeat this operation for all other dimensions. Confirm the sketch by clicking on the button. Note: If you want to cancel all that has been created or modified in the sketch, click on the red cross icon. A message will display, asking you to confirm the cancellation. Missler Software 3

10 Exercise 1: The axis sketch TopSolid Design Basics Modifying the sketch Edit the sketch by right-clicking on one of the segments, then selecting the Edit function. Create the new contour shown below by clicking on the previous contour for points G and K. Once point K has been created, tell TopSolid that the contour is open by right-clicking and selecting OK. Note: TopSolid automatically creates coincidence constraints on points G and K. The two green circles shown on the picture above tell the user that the contour is open. Trim the first contour by clicking on the GB segment, and then on the BK segment. Note: In the 1 st method described above, you have removed the GB segment first, and then the BK segment. By enabling the Profile option, you would remove both the GB and BK segments at once by clicking just one of them. 4 Missler Software

11 TopSolid Design Basics Exercise 1: The axis sketch Finish dimensioning the sketch in order to obtain the contour below. Confirm the changes made to the sketch by clicking on the button. Save, then close the document by using the mouse wheel on the part document s upper tab. NOTES Missler Software 5

12 Exercise 2: The second sketch TopSolid Design Basics Exercise 2: The second sketch Concepts addressed: - Creating circular geometric entities - Creating a tangent arc - Creating a sketch by trimming - Using construction geometries Creating a new part document In the Project tree, right-click on the project name and create a new Part document. Select Blank Template and click on to confirm. Rename the part Second Sketch and validate by pressing the Enter key. Creating the sketch In the 2D Sketch tab, create a circle with a diameter of 110mm and place its center on the frame s origin. Note: The circle should be blue because it is fully constrained in its dimension and position. 6 Missler Software

13 TopSolid Design Basics Exercise 2: The second sketch Create a second circle 30mm in diameter, whose center point is positioned without constraint anywhere to the top right of the first circle. Note: The Ø30mm circle will be pink because it is not constrained to its position. Create a third circle 60mm in diameter, whose center point is positioned on the X axis. Add the dimension of 150mm as seen in the picture below. Draw a line from the absolute origin point to the center of the Ø30mm circle and constrain this line as seen below. Reminder: The circle is blue because it is fully constrained in its dimension and position. Note: The line that has just been drawn simply positions the Ø30mm circle and should not be used to create the shape of the part. That is why the line has the status of a "construction line". Missler Software 7

14 Exercise 2: The second sketch TopSolid Design Basics Right-click on the line and select the Construction function. Make an arc tangent to the three circles created before, starting with the Ø30, then the Ø60, and ending the selection with the Ø110. The arc should be created in Free Size mode, and the Given Center option should not be checked. 8 Missler Software

15 TopSolid Design Basics Exercise 2: The second sketch Make an arc R70mm tangent to the Ø110 and Ø30 circles. Create an arc 150mm in diameter and tangent to the Ø110 and Ø60 circles. Missler Software 9

16 Exercise 2: The second sketch TopSolid Design Basics Trim the sketch to produce a closed contour. Note: You may repeat the trim operation in Delete selected part mode several times on successive arcs in the same circle. Confirm the sketch by clicking on the button. Save and close the document. NOTES Missler Software

17 TopSolid Design Basics Exercise 3: The bracket Exercise 3: The bracket Concepts addressed: - Adding constraints - Extruding a contour - Performing a volume trim - Making a drilling - Assigning properties - Generating a draft document - Creating views Creating a new part document In the Project tree, right-click on the project name and create a new Part document. Choose Blank Template and click on to confirm. Rename the part The Bracket and validate by pressing the Enter key. Creating a sketch by points Use the Contour function to create a profile by points, starting anywhere in the graphical area. Note: To create the circle's arc tangent to point F, we will indicate that we intend to design it by passing over point F several times with the mouse pointer. Depending on how you pass the mouse pointer over, TopSolid asks if the segment to be drawn is either a line segment or an arc segment and if it is normal, tangent, or perpendicular. Constrain the circle s arc FG and the segment GH in tangency. To do this, right-click on point G and select Tangent. Create a coincidence constraint on point C with the origin point of the absolute frame. To do this, click on point C and keep the left button pressed while moving toward the frame's origin. Release the left button when the origin is selected. Dimensionally constrain the contour to obtain the result shown opposite. Confirm the sketch by clicking on the button. Missler Software 11

18 Exercise 3: The bracket TopSolid Design Basics Creating the part Click on the Shape tab. Extrude the sketch 1 along Z+ to a height of 10mm. Validate the extrusion. Save the part document. Note: To move a sketch, you have the following two options: - on a geometry: The geometry and everything associated with it moves. - Alt key + on a geometry: All geometries that make up the contour move. Drafting the part Creating the draft document Right-click on the document window's upper tab Draft function. and select the Open the Standard Templates United States folder, choose the Part A4 ISO Portrait template, then click on confirm. to 12 Missler Software

19 TopSolid Design Basics Exercise 3: The bracket Creating the main view Once the draft document has been generated, TopSolid automatically creates a main view. In the Main View dialog, select Bottom Camera in the drop-down list and click at the top left of the drawing to position the main view. Orient the view using the blue arrow sphere so that your view matches the main view shown below. Validate the main view. TopSolid then proposes to create auxiliary views. Missler Software 13

20 Exercise 3: The bracket TopSolid Design Basics Creating the left view Click to the right of the main view in the drawing to create the following left view. Creating the perspective view In the Scale dialog, enable the Relative to Drafting option and set the scale factor to 0,8. In the Lines dialog, in the Hidden Lines section, select Hidden in the dropdown list. In the Render mode dialog, select Shading in the drop-down list. Click at the bottom right of the draft to put the perspective shading view. Finish the view projection by clicking on the icon. If necessary, reposition the views by moving them with the mouse cursor so as to obtain the draft shown opposite. Save the draft document. 14 Missler Software

21 TopSolid Design Basics Exercise 3: The bracket Creating a new sketch in the part document Click on the Bracket part document's upper tab to make the document current. In the 2D Sketch tab, create a new rectangle. In the drop-down list, select Absolute XY Plane as the sketch's support plane and click on to confirm. Note: TopSolid automatically creates the sketch 2. Draw the rectangle seen opposite by clicking on the first point of the part s vertical edge coinciding with the Y axis. Constrain the rectangle as seen opposite. Confirm the sketch by clicking on the button. Right-click on sketch 2 and select Trim by Profile. Check that the arrow points towards the side to be deleted. If not, double-click on the arrow to reverse its direction. Validate the trimming operation. In the Shape tab, select the Drilling function. Now we will drill a smooth Ø32mm through hole that is concentric to the part's cylindrical face Position the mouse cursor on the part s upper face while moving towards the cylindrical face. TopSolid interprets that the drilling is concentric to the fillet. Left-click to confirm the proposed positioning. Missler Software 15

22 Exercise 3: The bracket TopSolid Design Basics In the Hole dialog, set the diameter to 32mm and enable the Through option Validate the drilling. Assigning properties In the Project tree, right-click on the part document The bracket and select Properties. Click on the Edit button. Enter the following properties: - Description: Bracket - Part number: EX03 16 Missler Software

23 TopSolid Design Basics Exercise 3: The bracket Validate the properties. Note: The Description and Part number properties are document parameters that can be found in the Parameters folder of the Entities tree. Save the part document. Click on the Bracket draft document's upper tab to make the document current. Following the changes made to the part document, TopSolid has automatically updated the related draft document. In this way, the part document properties are automatically completed in the draft s title block. Save and close all documents. Missler Software 17

24 Exercise 4: The clamp TopSolid Design Basics Exercise 4: The clamp Concepts addressed: - Putting part knowledge to use: sketch, extrusion, drilling, trimming - Creating a chamfer and fillets - Putting draft knowledge to use: main view, auxiliary view and perspective view - Dimensioning a drawing 18 Missler Software

25 TopSolid Design Basics Exercise 5: The handle Exercise 5: The handle Concepts addressed: - Extruding a contour up to - Creating a revolved shape - Creating a tapped hole - Creating fillets - Creating a boss - Hiding/Showing elements - Modifying attributes - Declaring the design representation Creating a new part document In the Project tree, right-click on the project name and create a new Part document Choose Blank Template and click on to confirm. Rename the part The handle and validate by pressing the Enter key. Creating the first sketch Create a Ø50mm circle on the frame s origin. Create a Ø13mm circle and position its center at the intersection of the Ø50 circle and the Y+ axis. Repeat this operation three times to produce the result seen below. Warning: Do not use the 2D Sketch > Operations > Repetition command because the repetition would be after the resolution of the sketch in the sequence of operations. Missler Software 19

26 Exercise 5: The handle TopSolid Design Basics Create a new circle in Free size mode. The center of the circle is the frame's origin point, and the passing point is one of the Ø13 circles. Note: TopSolid automatically creates a tangency constraint with the Ø13 circle. Hold down the Ctrl key and select the two circles centered on the origin. Right-click in the graphical area and select the Construction function. Create an arc in Free size mode. Uncheck Given Center in the dialog and click on points A, B and C one after the other. 20 Missler Software

27 TopSolid Design Basics Exercise 5: The handle Repeat the operation to obtain the following result. then Trim the sketch to produce a closed contour. Complete the dialog box with the following parameters, click on the parts of the Ø13 circles to keep. Confirm the sketch by clicking on the button. In the visualization and rendering bar to the right of the graphical area, switch to Perspective camera by clicking on the icon. Missler Software 21

28 Exercise 5: The handle TopSolid Design Basics Creating the second sketch Click on the Arc icon. Select Absolute XZ Plane as the support plane in the drop-down list, and then click on confirm. to Create the R50mm arc positioned by any two points D and E. Note: The order in which the points are designated determines the convexity (trigonometric direction) or concavity of the arc (anti-trigonometric direction). Drag the point D over the X axis to constrain it in coincidence. Drag the point E over the Y axis to constrain it in coincidence. Perpendicularly constrain the Y axis and the arc to point E. Add the dimension of 14mm. Confirm the sketch by clicking on the button. 22 Missler Software

29 TopSolid Design Basics Exercise 5: The handle Creating the revolved surface Create a revolved shape by right-clicking on the previously created sketch and selecting Revolved. Modify the default revolution axis and select Absolute Z Axis in the drop-down list. Validate the revolved shape. Creating the extruded shape up to the surface Right-click on the surface and select Attributes in the Shape 1 section. Missler Software 23

30 Exercise 5: The handle TopSolid Design Basics Change the color of the surface to yellow, then click on to confirm. Extrude sketch 1 up to the previously created surface. To do this, right-click on sketch 1 and select the Extruded function. In the Limit field, select Surface in the drop-down list, then click on the yellow surface. Validate the extrusion. 24 Missler Software

31 TopSolid Design Basics Exercise 5: The handle Hide the yellow surface by right-clicking on the surface and selecting Hide in the Shape 1 section. Similarly, hide the sketch 1. Creating the third sketch Right-click on the part's lower face and select Sketch. Create a Ø20mm circle centered on the frame s origin. Confirm the sketch by clicking on the button. Creating the boss Right-click on sketch 3 and select Boss. Missler Software 25

32 Exercise 5: The handle TopSolid Design Basics In the dialog, complete the following fields: - Select Height as the limit and enter 15mm. - Check the Draft box and enter 8. Enable the Blend and Fillets dialog. Select Fillet as the blend type in the drop-down list and set the radius value to 2mm and the top radius to 0,5mm. Validate the boss. 26 Missler Software

33 TopSolid Design Basics Exercise 5: The handle Creating the tapped hole Create a M8 tapped hole with a depth of 10mm on the upper face of the boss. To do this, right-click on the upper face of the boss and select Drilling. Enable the Tapped hole mode. Open the Tapped hole dialog. Set the nominal diameter to 8mm. TopSolid automatically determines the pitch and the description values (Metric ISO 724 standard). Uncheck the True box to get the False value, then set the tapping depth to 10mm. Validate the drilling. From the Shape tab, make fillets on the part s sharp edges using the icon. Check the Different box in the dialog. Set the radius to 3mm and click on the part s upper edge. Then modify the radius value to 1mm and click on the part's lower edge. Validate the fillets. Missler Software 27

34 Exercise 5: The handle TopSolid Design Basics Declaring the part representation Note: The first shape created in a TopSolid document is considered to be the part being created. However, this is not so in this exercise, since the first shape generated here was the yellow surface, which is used only to perform a trim. TopSolid must therefore be told that the part we want is not the yellow surface, but the solid. Display the Entities tree. To do this, click on the TopSolid 7 icon and select View > Entities. In the Entities tree, open the Representations folder. In Design Representation, right-click on Shape 1 and select Delete. Do the same for Detailed Representation. Open the Shapes folder and drag Shape 2 into Design Representation. Do the same for Detailed Representation. Assigning properties In the Project tree, right-click on the part document The handle and select Properties. Click on the Edit button. Enter the following properties: - Description: Handle - Part number: EX05 Confirm the properties. Save the document. 28 Missler Software

35 TopSolid Design Basics Exercise 5: The handle Drafting the handle Creating a new draft Right-click on the part document s upper tab and create a new draft. Open the Standard Templates - United States folder, choose the Part A4 ISO Portrait template and click on to confirm. TopSolid automatically renames the draft document as the related part document. Create the draft shown below by following the method explained in the previous exercises. Missler Software 29

36 Exercise 5: The handle TopSolid Design Basics Making a cross section In the View tab, select the Cross Section function, choose the front view as the reference view, then select Standard as the cross section type. Validate by clicking on the blue arrow icon. Enable the Vertical mode and select the top of the drilling s cone to position the cross section polygon. If necessary, invert the direction of the cross section by double-clicking on the arrow s yellow handles. Validate the cross section polygon by clicking on the button. Position the view as seen below. Confirm the cross section view. 30 Missler Software

37 TopSolid Design Basics Exercise 5: The handle Activate the Exact Projection mode. Save the document. Missler Software 31

38 Exercise 6: The flange TopSolid Design Basics Exercise 6: The flange Concepts addressed: - Creating a parallel profile - Using a symmetry constraint - Creating a pocket - Repeating an operation - Modifying an operation Creating a new part document In the Project tree, right-click on the project name and create a new Part document. Choose Blank Template and click on to confirm. Rename the part The Flange and validate by pressing the Enter key. Creating the sketch Create a circle 60mm in radius centered on the origin. Create an offset to the X axis at a distance of 45mm from Y+. Draw an oblique line passing through the origin. Add the dimension of 65mm and the angle of 20. Right-click on the oblique line to give it the status of a construction line. Create three Ø20mm circles positioned as shown opposite. Create all of the missing lines to produce the following sketch. 32 Missler Software

39 TopSolid Design Basics Exercise 6: The flange Trim the sketch to produce a closed contour. Confirm the sketch by clicking on the button. Save the document. General settings for the sketch These settings can be enabled or disabled at any point in the design: - Activate the magnetic grid - Create the geometry in construction mode - Project the geometry in the plane - Automatically place dimensions on some geometric entities - Activate asking for the dimension value when placing it - Activate automatic relations between geometric entities - Activate the automatic alignment of geometric entities - Show/Hide the sketch's internal elements - Show/Hide the sketch's relations - Show/Hide extremities in the sketch - Create a cut with respect to the active plane Missler Software 33

40 Exercise 6: The flange TopSolid Design Basics Creating the shape In the Shape tab, extrude the sketch 1 to a height of 10mm along Z+. Right-click on the side edge shown below and make a fillet of 8mm Validate the creation of the fillet. Creating operations on the shape Right-click on the flange s upper face and create a new sketch. Make a R55mm circle centered on the origin. Right-click in the graphical area and make a boss with a height of 8mm, then click on to confirm. 34 Missler Software

41 TopSolid Design Basics Exercise 6: The flange The result should be as follows: Right-click on the top face of the boss and create a new sketch. Create a contour by observing the creation order seen below. The circle s arc will be created using the Arc mode. Constrain in coincidence the point 2 with the X axis. Dimension the contour as seen opposite. To create a symmetry on the angle, right-click on the value 120, select the X axis. Define Centering, then click on Add a concentricity constraint between the R50mm arc and the boss diameter. Missler Software 35

42 Exercise 6: The flange TopSolid Design Basics Right-click in the graphical area and create a 6mm deep pocket with respect to the upper face. Enable the Blend and Fillets dialog. Select None as the blend type in the drop-down list, then set the bottom radius to 2mm and the vertical radius to 10mm. Validate the pocket. Right-click inside the pocket and perform a repetition (Others > Repetition) using a circular pattern. Validate the circular pattern, and then the repetition. 36 Missler Software

43 TopSolid Design Basics Exercise 6: The flange Using the Drilling function from the Shape tab, make three smooth Ø10mm through holes with axes on the flange s three radii. Validate the drillings. Modifying the pocket sketch Right-click on the pocket and select Edit Sketch. Modify the pocket sketch in order to produce the contour shown opposite. Warning: Place the dimension of 6mm before deleting the arc portion using the Trim function. Validate the sketch by clicking on the button. Note: Validating the sketch will automatically make changes to the shape. Assigning properties In the Project tree, right-click on the part document The flange and select Properties. Click on the Edit button. Enter the following properties: - Description: Flange - Part number: EX06 Confirm the properties. Missler Software 37

44 Exercise 6: The flange TopSolid Design Basics Modifying one of the drillings Right-click on the lower smooth hole and replace it with a 5mm deep Ø16mm spot-faced hole and with a Ø10mm through hole. Save and close the document. 38 Missler Software

45 TopSolid Design Basics Exercise 7: The key Exercise 7: The key Concepts addressed: - Create a regular polygon - Create a pipe operation - Using entities - Using Boolean operations Creating a new part document Right-click on the project name and create a new Part document. Choose Blank Template and click on to confirm. Rename the part The Key and validate by pressing the Enter key. Creating the sketch Create a new sketch on the absolute XY plane. Draw the contour shown below, and then add the geometric and dimensional constraints. Confirm the sketch by clicking on the button. Create a new sketch on the absolute ZX plane and build a R19mm circle on the plane s origin. This circle will be used later. Confirm the sketch by clicking on the button. Create a new sketch on the absolute ZX plane and create two regular polygons with 6 vertices on an inner diameter of 25,5mm. For the first polygon, click on the frame s origin, then on the X axis. For the second polygon, click on the frame s origin, then on the Y axis. If necessary, modify the angular dimensions to produce the result shown opposite. Confirm the sketch by clicking on the button. Missler Software 39

46 Exercise 7: The key TopSolid Design Basics Right-click on each created sketch and select the Attributes function to assign them a different color. Create a new sketch on the absolute ZX plane and build a rectangle constrained as below. Confirm the sketch by clicking on the button. Note: To make it easier to use the sketches, it may be useful to rename them. To do this, simply go to the Sketches folder in the Entities tree and rename them one by one. To rename any element in a tree, you can either click twice on the element at one-second interval and enter the new name, or click on the element, press the F2 key and enter the new name. The result may be the following: 40 Missler Software

47 TopSolid Design Basics Exercise 7: The key In the Tools tab, create a plane by point and normal from the right end of the Handle sketch and normal to the Y axis. Create a new sketch on the created plane, then rename it Circle R12,5. Make a R12,5mm circle on the end of the handle profile. Validate the Circle R12,5 sketch. Change the color of the sketch using the Attributes contextual command. Create a new sketch on the same plane and rename it Square. Build a 12,7 x 12,7mm centered square. Validate the Square sketch. Missler Software 41

48 Exercise 7: The key TopSolid Design Basics Change the color of the sketch using the Attributes contextual command. Build a plane by point and normal from the end of the Handle sketch and normal to the X axis. Create a new sketch on the created plane and rename it Handle section. Build a rectangle constrained as below. Confirm the Handle section sketch. Change the color of the sketch using the Attributes contextual command. Hide the two created planes. 42 Missler Software

49 TopSolid Design Basics Exercise 7: The key Creating the shape In the Surface tab, create a pipe using the Handle sketch as the path and the Handle section sketch as the section. Validate the pipe. Extrude the Circle R19 sketch by aligning it centered on 12,5mm, then validate the extrusion. Change the color of the cylindrical shape using the Attributes contextual command. Create a new sketch on the inner face of the cylinder. Create a 2mm offset inside of the shape's circular sketch. Missler Software 43

50 Exercise 7: The key TopSolid Design Basics Make a 4mm in height boss with a draft of 5. Extrude the Polygons sketch in Center mode to 30mm and click on. Extrude the Rectangle for slot sketch in Center mode to 30mm and click on. Extrude the Circle R12,5 sketch in Center mode to 15mm and click on. Extrude the Square sketch in Center mode to 20mm and click on. Give each shape a different color. In the Shape tab, click on the Boolean icon and unite the shape from the Polygons sketch with the one from the Rectangle for slot sketch by enabling the Union mode. Similarly, unite the shape from the Handle sketch with the one from the Circle R19 sketch and the one from the Circle R12,5 sketch. 44 Missler Software

51 TopSolid Design Basics Exercise 7: The key The result is a part comprising three shapes: Always with the Boolean function, subtract the green shape and the yellow shape (these two are tools) from the gray shape by enabling the Subtraction mode. The result must be the following: The different Boolean operations: Subtraction: Union: Intersection: Edit the Handle sketch and add 10mm fillets by clicking on the icon from the 2D Sketch tab. This produces the result shown opposite. Missler Software 45

52 Exercise 7: The key TopSolid Design Basics Assigning properties In the Project tree, right-click on the part document The key and select Properties. Click on the Edit button. Enter the following properties: - Description: Key - Part number: EX07 Confirm the properties. Save and close the document. NOTES Missler Software

53 TopSolid Design Basics Exercise 8: The roller Exercise 8: The roller Concepts addressed: - Putting knowledge to use 1. Creating a new part document Right-click on the project name and create a new Part document. Choose Blank Template and click on to confirm. Rename the part The roller and validate by pressing the Enter key. Creating the sketch Create three circles as seen below. Create two arcs with a 47mm radius and two others with a radius of 16mm as seen below. Position the arc without worrying about its direction or concavity, then right-click on the arc and select the Symmetric and/or Complementary options to produce the desired arc. Missler Software 47

54 Exercise 8: The roller TopSolid Design Basics Note: If you want to change the visualization tolerance so that your circles do not look like polygons, the visualization button on the bottom right corner of the screen: click on Warning: Adjust the tolerance by finding the right balance between visual accuracy and PC performance because the finer the tolerance, the more accurate and better your representation will be, but more resources will be needed to display the rendering. Trim the sketch to produce a closed contour. Creating the shape Right-click in the graphical area and extrude the 10mm sketch by enabling the Center mode. Validate the extrusion. Make the two smooth Ø10 through holes with axes on the far two radii. Validate the drillings. Right-click on the top face of the roller and create a new sketch. Create a circle with a 20mm radius centered on the origin. 48 Missler Software

55 TopSolid Design Basics Exercise 8: The roller Create a boss from the circle by completing the fields as below, then click on to confirm. Repeat the boss using a plane symmetrical pattern in relation to XY. Validate the repetition. and Create a Ø30 through hole in the center of the boss validate the drilling. Add 2mm fillets to the part's outer edges and validate the fillets. Missler Software 49

56 Exercise 8: The roller TopSolid Design Basics Right-click on the part and change its color using the Attributes function. In the Entities tree, open the Sketches folder, rightclick on Sketch 1 and select Show. In the graphical area, right-click on sketch 1 and select Others > Pipe. Note: We will reuse an existing sketch (Sketch 1) to create another shape, which will be used to modify the original shape. Enable the Wire shape mode and set the diameter to 3mm. The preview should look as follows: Validate the pipe. The result is therefore a part comprising two shapes. This result can be seen in the Entities tree. Note: The goal is to create a circular slot in the original shape. 50 Missler Software

57 TopSolid Design Basics Exercise 8: The roller In the Shape tab, use the Boolean function and select the Subtraction mode. Note: The original shape (Shape 1) is to be modified and the pipe (Shape 2) is the subtraction tool. Validate the subtraction. Assigning properties In the Project tree, right-click on the part document The roller and select Properties. Click on the Edit button. Enter the following properties: - Description: Roller - Part number: EX08 Confirm the properties. In the Project tree, open the References node and check that the TopSolid Mechanical library is visible. In the Tools tab, select the Material and Coating function. In the dialog, uncheck No Material, select Copper Alloys as the category and Brass as the material, and then click on to confirm. Missler Software 51

58 Exercise 8: The roller TopSolid Design Basics Always in the Tools tab, select the Physical Properties function. Open the Mass dialog, check the Automatic option, then click on to confirm. Check that the material has been successfully added to the Entities tree. The Brass material should appear in the part's Parameters folder Save and close the document. 52 Missler Software

59 TopSolid Design Basics Exercise 9: The roller draft Exercise 9: The roller draft Concepts addressed: - Choosing the drafting format - Creating the detail views - Placing the axes - Dimensioning Creating the draft document Create a new Draft document using the Part A4 ISO Landscape template and click on to confirm. Rename the draft The roller and validate by pressing the Enter key. Right-click on the drawing s border and edit it. From this window, it is then possible to change the format of the drawing. Click on to confirm. Creating the main view and auxiliary views Drag the part document The roller into the draft. Position the main view as seen in the image below. Then create the top view and the perspective view as seen below. Missler Software 53

60 Exercise 9: The roller draft TopSolid Design Basics In the Detailing tab, select Automatic Axes to place the axes on the main view. Dimension the different views. Add text to indicate the fillets on the perspective. Save and close the document. Modifying the part The roller Open the part document The roller. Right-click on the top face of the roller and create a new sketch. 54 Missler Software

61 TopSolid Design Basics Exercise 9: The roller draft Create a rectangle and constrain it as seen opposite. Trim the roller using a profile. Validate the trimming operation. Save and close the document. Updating the draft and adding detail views Open the draft document and check that it has been correctly updated. Make two detail views at a 2:1 scale on the key slot and on the boss. To do this, go to the View tab, select Detail View and click on the reference view. You go into a sketch which allows you to define the circle delimiting the area to be detailed. Enter the desired radius and click on a center point. Click on the button to confirm the detail sketch. Position your detail view and click on to confirm. Save and close the document. Missler Software 55

62 Exercise 10: The cam TopSolid Design Basics Exercise 10: The cam Concepts addressed: - Putting knowledge to use 2. Notes: - The centers of the circles with a radius of 90mm and 80mm are at the end of a 12mm line that makes a 45 angle with the X axis. - The undimensioned radii are 10mm (see note above the title block). - For the first tapping, create a frame by point and 2 directions and repeat the operation 8 times with a spacing angle of In the Operations tree, right-click on the repetition, use the Exclusion function and select the copies to delete. 56 Missler Software

63 TopSolid Design Basics Exercise 11: The axis Exercise 11: The axis Concepts addressed: - Creating a groove - Creating chamfers - Performing a partial trimming Creating a new part document Right-click on the project name and create a new Part document. Choose Blank Template and click on to confirm. Rename the part The axis and validate by pressing the Enter key. Creating the sketch Create the following contour in a new sketch. In the Shape tab, create a revolved shape of 360 around the X axis. Validate the revolved shape. Always in the Shape tab, select the Groove or Shoulder function and create a groove. Open the Section dialog and select the Shifted Rectangle model in the drop-down list. Open the Drivers dialog and set the offset and width values to be 3mm. Missler Software 57

64 Exercise 11: The axis TopSolid Design Basics Open the Position dialog and complete the fields as follows: - Click in the Axial Frame field to move the cursor there, then click on the planar face at the end of the part as seen below. - Modify the position of the groove with respect to the frame indicated by the label to 3mm. Validate the groove. Make two chamfers of 2mm at 45. Validate the chamfers. 58 Missler Software

65 TopSolid Design Basics Exercise 11: The axis Use the Shape > Drilling command to create a Ø38mm H7 boring along the part's rotation axis. Open the Hole dialog and complete the fields as follows: - Set the diameter to 38mm. - Click on the icon to the right of the field. - Select Tolerance > Hole > H7. - Enable the Through All mode. Validate the drilling. Create a M5 tapped hole with a depth of 12mm positioned by means of a polar frame. Validate the creation of the frame, then the drilling. Missler Software 59

66 Exercise 11: The axis TopSolid Design Basics Use the Shape > Repetition command to propagate the tapped hole using a circular pattern so as to obtain four tapped holes every 90. Create a new sketch on a 45 pivoted plane around the X axis. Create a Ø100mm circle with the center coordinates of: (90,50). Confirm the sketch by clicking on the button. 60 Missler Software

67 TopSolid Design Basics Exercise 11: The axis Use the Shape > Trim by Profile command to perform a partial trimming of 1mm from each side of the circle. Validate the trimming operation. Create a Ø3mm through hole positioned by means of a radial frame whose reference plane is the planar crown drilled with four tapped holes. Click on the icon to reverse the normal direction for this reference plane. Validate the creation of the frame, and then the drilling. Assigning properties In the Project tree, right-click on the part document The axis and select Properties. Click on the Edit button. Enter the following properties: - Description: Axis - Part number: EX011 Confirm the properties. Save and close the document. Missler Software 61

68 Exercise 12: The elbow TopSolid Design Basics Exercise 12: The elbow Concepts addressed: - Projecting a sketch - Thickening a surface - Repositioning the origin of a frame Creating a new part document Create a new Part document using a blank template and click on to confirm. Rename the part The elbow and validate by pressing the Enter key. Creating the sketch Make a Ø180mm circle centered on the origin. Create the following sketch and add the dimensional and geometric constraints. Note that the R200mm arc and the Ø180mm circle are concentric. Trim the segments to produce the profile shown below. 62 Missler Software

69 TopSolid Design Basics Exercise 12: The elbow Confirm the sketch by clicking on the button. Create a new sketch on the absolute XY plane and draw the following profile. Add the dimensional and geometric constraints as seen below. Confirm the sketch by clicking on the button. Extrude the sketch 1 to 25mm along Z- and click on to confirm. Change the color of the part. Missler Software 63

70 Exercise 12: The elbow TopSolid Design Basics Make R20 and R40 fillets on vertical edges of the sole as seen below, and click on to confirm. Make a pocket on the inner face of the sole according to the parameters below. Warning: The reference plane will be the inner face of the sole as it appears below with the part turned over to directly show the pocket. Validate the pocket. 64 Missler Software

71 TopSolid Design Basics Exercise 12: The elbow Make a Ø150mm through hole on the face of the sole. Validate the drilling. Create a new sketch on the top face of the sole. In the 2D Sketch tab, click on the Project icon and project the circular edge of the drilling onto the current sketch plane. Validate the projection. Confirm the sketch by clicking on the button. Create a new sketch on the absolute YZ plane. Missler Software 65

72 Exercise 12: The elbow TopSolid Design Basics Create a R200mm circle s arc passing through the center point of the drilling and a second point positioned anywhere. Add a coincidence constraint between the center point of the arc and the X axis. Draw a construction line between the center of the arc and the second end of the arc. Finish adding the dimension of 30. Confirm the sketch by clicking on the button. Create a pipe with the arc as the path and the circle as the section. Check the Surface box so that the pipe is only a surface. Validate the piped shape. 66 Missler Software

73 TopSolid Design Basics Exercise 12: The elbow Note: At this point, your part is comprised of two separate shapes. The sole is solid, and the pipe is a surface. A thickening operation will transform the surface shape of the pipe into a solid, which will then be able to unite with the sole's solid shape. In the Shape tab s drop-down menu, select Other Operations > Thickening and thicken the pipe surface outward by 8mm. Validate the thickening operation. Unite the two solids and click on to confirm. Make a 10mm fillet where the two solids join and click on to confirm. Missler Software 67

74 Exercise 12: The elbow TopSolid Design Basics Create a new sketch on the top face of the elbow. Position the plane's origin point at the center of the elbow's top face by selecting one of the two circular edges, then click on confirm the positioning. Project the inner circular edge of the elbow and click on to confirm the projection. to Build a 186x186mm rectangle centered on the origin. Confirm the sketch by clicking on the button. Make a 10mm high boss with vertical radii of 20mm. Validate the boss. 68 Missler Software

75 TopSolid Design Basics Exercise 12: The elbow Make a M10 tapped through hole that is concentric to a vertical fillet of the boss. Repeat this hole with double plane symmetry. Note: Warning on symmetry planes: The first will be the YZ plane, and the second will be the middle plane of the two inclined faces of the boss. Assigning properties In the Project tree, right-click on the part document The elbow and select Properties. Click on the Edit button. Enter the following properties: - Description: Elbow - Part number: EX012 Confirm the properties. Save and close the document. NOTES Missler Software 69

76 Exercise 13: The puncher TopSolid Design Basics Exercise 13: The puncher Concepts addressed: - Creating a new assembly document - Inserting a part into the assembly - Creating an in-place part in the assembly - Importing a TopSolid component into the assembly - Importing a Parasolid component into the assembly Create a new Part document using a blank template and click on to confirm. Rename the part The body and validate by pressing the Enter key. Creating the body Creating the initial shape Create a new sketch and build the following profile. Add the dimensional and geometric constraints as seen below. on Extrude the sketch to a height of 38mm by centering the shape with respect to the sketch plane and click to confirm. 70 Missler Software

77 TopSolid Design Basics Exercise 13: The puncher Turn the part to a position similar to what is shown in the image below. Then right-click on the bottom face of the extruded shape and select View Along Normal. Display the Entities tree and open the Cameras folder. Right-click on Front Camera, select Define From View and validate View 1. Click on the side icon to select the perspective camera. Create a new sketch on the part s inclined face. Build a rectangle constrained as seen below. Note: If the distance dimensions between the sides of the rectangle and the edges of the oblique face appear between parentheses, the dimensions have been disabled because they are redundant with the rectangle's general dimensions. You should therefore delete the rectangle's general dimensions and then enable the dimensions in parentheses using the contextual menu for those dimensions. You can then modify their value. Create a pocket with a depth of 4mm, vertical radii of 8mm and a 1mm bottom radius. Validate the pocket. Missler Software 71

78 Exercise 13: The puncher TopSolid Design Basics Inserting an operation into the construction tree Right-click on the pocket in the graphical area and select Others > Insert Before. This command is used for inserting one or more operations before the selected operation. In this case, the goal is to create two fillets on the top and bottom edges of the inclined face. Create the two R4mm fillets on the two edges seen above. The Operations tree shows all of the operations for the current document, in the order in which they were created. It also allows you to insert and swap operations. Moreover, the Operations tree, just like the Entities, the Parts and the Options trees, provides a quick search function to filter the elements, based on the text you entered in the input field. You just have to click on the icon to display the search field. Finishing the insertion To indicate that you do not wish to insert any other operations after the fillet, you have two options: Return the insertion cursor ( Modeling Stage) in the Operations tree to the top. Or, even easier, click on the insertion cursor to the right of the part document s upper tab. Your subsequent operations will now be carried out after the pocket. 72 Missler Software

79 TopSolid Design Basics Exercise 13: The puncher Make a Ø12 H7 boring on the top face as seen below. Select Constrained Frame in the special inputs for creating a frame and complete the fields as below. Validate the creation of the frame, and then the drilling. Missler Software 73

80 Exercise 13: The puncher TopSolid Design Basics Create four R10mm fillets on the front of the part and another R1mm fillet along the edge leading from the top face of the part. Enter the following part properties: - Description: Body - Part number: P01_01 - Material: Aluminum Save and close the document. Creating the assembly document In the Project tree, right-click on the project name, create a new Assembly document using a blank template and click on to confirm. Rename the assembly document The puncher. Drag the part document The body into the assembly document The puncher. The part is automatically positioned so as to make the absolute frames of the part and assembly coincide. The constraint associated with the part is a fixity. The part and its constraint are visible in the Parts and Constraints folders in the assembly's Entities tree. The fixity constraint can be deleted or deactivated in order to manually move the part in the assembly. 74 Missler Software

81 TopSolid Design Basics Exercise 13: The puncher Creating the in-place sole select Right-click on the lower face of the body and In Place Part. Use a blank template and click on to confirm. A new part document is then created. Because the part is created "in place" in the assembly, the document is included in the assembly document node in the Project tree, and not outside of this node like the part document The body. Rename the new document for the part created in place to The sole. Create a rectangle constrained as seen below. Missler Software 75

82 Exercise 13: The puncher TopSolid Design Basics Extrude the sketch to 10mm and click on to confirm. Make a Ø6 H7 boring on the top face of the sole, positioned by means of an axial frame: - Click on the Z Axis icon. - In the Z Axis field, click inside one of the bored cylinders in the body of the puncher. If needed, click on the icon in front of the Z Axis field to point the arrow towards the outside of the sole. - In the Reference Plane field, click on the sole s top face. - Set the distance value to 0mm. - Enable the Orient X option. 76 Missler Software

83 TopSolid Design Basics Exercise 13: The puncher Make a Ø15mm hole with a depth of 5mm at the same place under the sole. The result will be a Ø6H7 spot-faced boring with Ø15mm and a depth of 5mm. Confirm the sole's in-place design by clicking on the button. Importing a Parasolid file In the Project tree, right-click on the project name or the folder where your puncher is located and select Import/Export > Import File with Conversion. Open the Punch+Pin.x_t file. Fill out the dialog box as shown opposite. Validate the import. Missler Software 77

84 Exercise 13: The puncher TopSolid Design Basics TopSolid displays the imported assembly in the graphical area and automatically creates a folder in the Project tree containing the parts that make up the assembly. Open the Punch part document and create a M8 threading on the upper cylindrical part. To do this, use the Shape > Threading command and do the following: - In the Face to thread field, click on the cylindrical face. - In the Origin plane field, click on the planar face above the cylinder. - In the Complete threading field, check the box for True. - Check the Standard option and select Metric ISO 724 in the drop-down list. - In the Description field, select M8 in the drop-down list. Validate the threading, then save and close the document. Make the Punch+Pin assembly document as current. TopSolid automatically propagates the part's threading to the assembly document. Using an asterisk, TopSolid notifies us that the change to the assembly document must be saved. Save and close the Punch+Pin document. Drag the Punch+Pin assembly into the assembly document The puncher. TopSolid 7 will specify the positioning constraints in terms of the geometry of the elements you indicate: - On the part to be positioned (Source) - On a part already included in the assembly (Destination) 78 Missler Software

85 TopSolid Design Basics Exercise 13: The puncher For the Punch+Pin document, do the following: - Source: Click on the punch's main cylindrical body. - Destination: Click on the Ø12H7 boring in the puncher. TopSolid 7 then proposes an Axis on Axis constraint. In the Assembly tab, now specify the type of constraint you wish to install by clicking on the Surface on Plane constraint icon. - Source: Click on the pin's cylindrical surface. - Destination: Click on the puncher body's planar face selected in the image shown opposite. Note: If needed, double-click on the icon to the left of the positioning label to invert the direction of the constraint in case the pin were to slide into the body of the puncher This Punch+Pin sub-assembly still has a degree of freedom, which allows it to turn freely around itself. To lock this rotation, we will use a plane for this sub-assembly that will be published. We will therefore quit the positioning sequence for this subassembly temporarily by clicking on the button. Missler Software 79

86 Exercise 13: The puncher TopSolid Design Basics We will return to this positioning once we have published the plane that we need. Save the document The puncher. Open the Punch+Pin assembly document. In the Punch+Pin document s Entities tree, open the Planes folder. Right-click on Absolute XY Plane and in the Selection section select Others > Publish Plane. In the dialog box, set the description to Plane, then click on to confirm the publishing. Save and close the document. 80 Missler Software

87 TopSolid Design Basics Exercise 13: The puncher Retrieving the publishing Make the assembly document The puncher current. Right-click on the Punch+Pin sub-assembly and select Publishings > Show Publishings. Now you see the plane you published. To go back to the positioning, use the Assembly > Plane on Plane command directly and complete the fields as follows: - Source: Click on the published plane. - Destination: Select the absolute XY plane in the drop-down list. Note: The sub-assembly changes to blue to indicate that it is fully constrained. Exit the sub-assembly positioning by clicking on the button Positioning the handle. Drag the part document The handle into the assembly document The puncher. Position the handle first using an Axis on Axis constraint. - Source: Click on the handle s M8 tapped hole. - Destination: Click on the punch's threading. Missler Software 81

88 Exercise 13: The puncher TopSolid Design Basics Place a second Plane on Plane constraint. - Source: Click on the handle's supporting face. - Destination: Click on the punch's shoulder face. Finish positioning the handle by adding a Plane on Plane constraint, whose source plane is the publishing of the absolute YZ plane from the document The handle, and the destination plane is the absolute XY plane from the assembly. Validate the positioning. Searching the libraries for a spring Let's search for a spring in the Vanel springs library. To search for the spring, the library must be referenced. In the Project Tree, open the References node and check that the TopSolid Vanel Springs library is present. If not, add it as described below. Right-click on References. Select Reference Library. Select TopSolid Vanel Springs in the list and click on to confirm. Open the search window by clicking on the TopSolid 7 icon and selecting View > Search. In the Search field, enter spring. In the Type field, select Family in the drop-down list. Specify to search in all projects. Run the search by clicking on the icon Refresh. 82 Missler Software

89 TopSolid Design Basics Exercise 13: The puncher From the list of families matching the search criteria, drag the Compression Spring with Ground Open Ends family into the Puncher assembly s graphical area. A wizard helps you position the correct spring. In the Wizard field, select Bottom Frame as the position frame in the dropdown list. In the Selected Part field, select the spring whose code is C A in the drop-down list. Open the Drivers dialog and set the spring length to 27mm. The type of spring has now been determined. It only needs to be positioned. Open the Positioning dialog. In the Bottom Frame field, click on the icon to create a frame on the fly. Use an axial frame and complete the fields as follows: - Z Axis: Click on the punch's cylindrical face and, if needed, invert the direction of the arrow to point upwards. - Reference Plane: Click on the top face of the body. - Orientation: Enable Orient X to coincide with the absolute Z axis. Validate the creation of the frame. Validate the inclusion of the spring. Missler Software 83

90 Exercise 13: The puncher TopSolid Design Basics By default, the spring is included in a simplified representation that makes only the top and bottom ends appear. To see the full spring, proceed as follows: Right-click on the spring and under the Compression Spring section select Others > Change Representation. Select Detailed Representation in the dropdown list. Validate the representation. Creating screws with their repeated drillings We will create drillings with the four corners of a rectangle on the bottom side of the puncher's sole. The rectangle will be created in a sketch that will determine the repetition pattern. Creating the sketch from the repetition pattern Start by making the body of the puncher semitransparent by selecting Attributes in the part s contextual menu. Create the sketch. To do this, right-click on the inner face of the sole and select Sketch. Create an offset profile located at 10mm from the lower edge of the body as seen in the image below. Make each point of the sketch not internal. Confirm the sketch by clicking on the button. 84 Missler Software

91 TopSolid Design Basics Exercise 13: The puncher Creating a screw and its drilling Run a search for screw families by entering screw in the Search field. From the list of screw families, drag the Hexagon Socket Head Cap Screw ISO 4762 family into the assembly document The puncher. - Wizard: Select Screw Buried Head in the drop-down list. - Selected Part: Select M4 x 12 in the drop-down list. The screw appears in the graphical area, ready to be positioned. Open the Positioning dialog. In the Top Frame field, click on the icon to create a frame on the fly. Use a frame by points and 2 directions and complete the fields as follows: - Origin: Click on the top-right vertex of the previously created rectangle. - X Direction: Select Absolute X Axis in the drop-down list. - Y Direction: Select Absolute Z Axis in the drop-down list. Validate the creation of the frame. Validate the inclusion of the screw. The wizard now asks you to use a process to create the drilling associated with this screw. In the Process field, select Tapped Hole in the drop-down list. Validate the process. A message then warns you that the body will be synchronized with the puncher. Click on OK. This means that the part document The body will be modified based on the assembly document The puncher and that any revision to either of these two documents will automatically revise the other document. These concepts will be explained in the following exercise. Missler Software 85

92 Exercise 13: The puncher TopSolid Design Basics Repeating the screw and drilling using a rectangular pattern In the Tools tab, repeat the screw using a sketch pattern. - Sketch: Select the sketch 1 of the rectangle. - Reference Point: Select Frame 2. Validate the repetition pattern. Validate the screw repetition. Validate the process repetition to produce the result seen below. Save the document. 86 Missler Software

93 TopSolid Design Basics Exercise 14: The PDM Exercise 14: The PDM Concepts addressed: - What is the PDM? - Project organization/structure of documents - Data backup/security/revision - Copying/Pasting a document - Deleting/Purging/Redirecting documents - Document life cycle (validated, design...) - History/Back references/references - Importing/Exporting a package The PDM (Product Data Management) helps to flexibly and securely store data about your projects. This data represents the backbone of your company, and it must be accessible to everyone as easily as possible. There are two options for connecting to a PDM server: in local mode or in client/server mode. Local mode The workspace is the area in which TopSolid users perform the document backups. The vault is a repository where documents are stored and secure. Missler Software 87

94 Exercise 14: The PDM TopSolid Design Basics Each document of the workspace is in a "new" state (symbolized by the is checked into the vault. The vaulting (symbolized by the and deletes the previous backups. icon) and keeps a backup history until it icon) validates the last state of the saved document The PDM allows you to manage the document revisions in a transparent way. In fact, each vaulting creates a new minor revision of the document. In this operating mode, data cannot be shared. Client/Server mode TopSolid users can connect to the server by using their own user account. The way of working is much the same as with the local PDM, with the ability to work as a team. Both PDM are therefore completely different. If you want to transfer documents or a project from the client/server mode to the local mode, you must export packages. Then you have to connect to the local PDM and import the package. Similarly, if you want to transfer documents or a project from the local mode to the client/server mode, you must export packages. Then, you have to connect to the PDM server and import the package. 88 Missler Software

95 TopSolid Design Basics Exercise 14: The PDM Project organization During training, all documents are created at the project root. We will now structure the project so that information can be found easily. Creating a folder in the project Right-click on the project name and select Folder. Rename the new folder 1-Design and validate by pressing the Enter key. Similarly, create a second folder and rename it 2-PDM. Creating three folders in 1-Design Right-click on the folder 1-Design. Create a new folder, rename it 1-Parts and validate by pressing the Enter key. Similarly, create a second folder named 2-Drafts and a third folder named 3-Assemblies. Missler Software 89

96 Exercise 14: The PDM TopSolid Design Basics Ordering the files within folders Drag all the parts created during the training into the folder 1- Parts. Note: To select multiple consecutive documents in the Project tree, use the Shift key +. To select multiple documents that are not consecutive, use the Ctrl key +. Repeat the operation for the drafts and assemblies so as to obtain the result shown opposite. Save the project. In order for the PDM exercise to be the same for all users, we will first import a package. Importing a package in the PDM folder A package is a set of documents stored in a single file whose extension is *.TopPkg. This package includes all the PDM information, which allows you to import/export a project (in whole or in part) without losing the links between the different documents of this project. In the Project tree, right-click on the folder 2-PDM. Select Import/Export, then Import Package. Open the file The Puncher.TopPkg on your hard disk. TopSolid indicates actions that will be performed. Confirm the import. 90 Missler Software

97 TopSolid Design Basics Exercise 14: The PDM The Project tree now includes the different documents that make up the puncher. These files are stored in the local PDM workspace. Document structure All file types have "major" and "minor" revisions. When created, a part has by default a major revision A, and a minor revision 0. Revisions help ensure the traceability of changes made to a document when checking in. However, major and minor revisions are the second step in the part tracking, whose functionalities will be discussed later. In fact, the first step is to save the different states of your document. Missler Software 91

98 Exercise 14: The PDM TopSolid Design Basics Using the file backup and its options First modification of the body Open the Body part document and change its color to red and its transparency to 50% using the Attributes function. Using an asterisk (*), TopSolid notifies us that a change has been made to the part document. Also notice that TopSolid has automatically created a Backups subfolder. Save and close the document. In the Project tree, note that the gray, non-transparent part that you previously imported has been added to the Backups subfolder. The new version of the red, transparent part is now A.0. Moreover, using the icon, TopSolid notifies us that the Puncher document is out-of-date. In fact, TopSolid has automatically redirected the new Body to the Puncher document. Consequently, TopSolid has to update the Puncher document to implement the changes. First update of the puncher Right-click on the Puncher assembly document. Select the Update function. Click on to confirm the update. 92 Missler Software

99 TopSolid Design Basics Exercise 14: The PDM Visualization of the parts in the Project tree Second modification of the body Modify the body a second time by changing its color to yellow and its transparency to 50%. Save and close the document. Second update of the puncher Update the Puncher document. Save and close the document. Where are the parts located in the Project tree? Missler Software 93

100 Exercise 14: The PDM TopSolid Design Basics Restoring a backup Right-click on the first backup of the body. Select Restore Backup. A window indicates that the restoration as latest A.0 revision is possible. Confirm the window. Update the Puncher document. Save and close the document. Where are the parts located in the Project tree? The gray body is shown twice in the Project tree; once as a saved part and once as an A.0 revised part. Similarly, the puncher with the gray body is shown twice; once as a saved assembly and once as an A.0 revised assembly. 94 Missler Software

101 TopSolid Design Basics Exercise 14: The PDM Where are the CAD files "physically" located? The CAD files are located in an area of your computer's hard drive called "workspace". The workspace is the area in which TopSolid users perform the file backups. Each document of the workspace is in a "new" state, which is symbolized by the icon. Each backup is stored in the Backups subfolder. If an error occurs, the user can restore a previous backup of the document as the current version. Local PDM Local PDM workspace Local vault Missler Software 95

102 Exercise 14: The PDM TopSolid Design Basics Data security We will now check the whole project into the vault. This will help keep data secure in an area called the "vault". Moreover, if you use a PDM server connection, this action allows you to make documents available to other users. Right-click on the project name and select Check In. A window indicates that listed documents can be checked into the vault. Click on to confirm. Where are the CAD files "physically" located? The CAD files are located in an area of your computer's hard drive called the "vault". Each document checked into the vault is symbolized by the icon. The vaulting allows you to secure the last saved version of your document. TopSolid assigns major and minor revisions, and then delete the backups. Local PDM Local PDM workspace Local vault Note that all documents for this project have been checked into the vault. Since it is the first time that these documents are checked in, TopSolid assigns them a major revision A, and a minor revision Missler Software

103 TopSolid Design Basics Exercise 14: The PDM Modifying a part We will now add four chamfers to the plate. In the Project tree, right-click on the Plate part document and select Check Out for Edit. A window indicates that the operation is possible. Click on to confirm. Where are the CAD files "physically" located? The CAD files that were previously created are still checked into the vault. The Plate part document is checked out for edit (the blue lock turns into a red check mark ). Moreover, TopSolid automatically creates a new Plate document in the workspace and assigns it a major revision A, and a minor revision 1. Two versions of the plate are now shown in the Project tree; the first revision (A.0) is in the vault and the second revision (A.1) is in the workspace. Local PDM Local PDM workspace Local vault Add four 10mm x 45 chamfers to the plate, and then select Check In. Missler Software 97

104 Exercise 14: The PDM TopSolid Design Basics Where are the CAD files "physically" located? Local PDM Local PDM workspace Local vault All documents are located in a secure zone called the vault. Using the icon, TopSolid notifies us that the Puncher document is out-of-date. TopSolid has automatically redirected the new plate with chamfers to the Puncher document. Consequently, TopSolid has to update the Puncher document to implement the changes made to the plate. Right-click on the Puncher document and select Update. Confirm the update. In the Project tree, the Puncher document has been updated and is now checked out (symbolized by the icon ). A new minor revision of the puncher has been created. 98 Missler Software

105 TopSolid Design Basics Exercise 14: The PDM Where are the CAD files "physically" located? Local PDM Local PDM workspace Local vault The Puncher document is checked out for edit (the blue lock turns into a red check mark ). TopSolid automatically creates a new Puncher document in the workspace and assigns it a major revision A, and a minor revision 1. Two versions of the puncher are now shown in the Project tree; the first revision (A.0) is in the vault and the second revision (A.1) is in the workspace. Data security Right-click on the project name and select Check In. A window indicates that the vaulting will only impact the Puncher document, since the other files are already checked into the vault. Note that you can add a comment when checking in one or more documents. This comment is recorded in the file history. Click on to confirm. Missler Software 99

106 Exercise 14: The PDM TopSolid Design Basics Where are the CAD files "physically" located? Local PDM Local PDM workspace Local vault All documents are now checked into the vault. Like the Plate document, the Puncher document has two revisions. The first revision (A.0) corresponds to the puncher without chamfers and the second revision (A.1) corresponds to the puncher with chamfers. Document history The History function allows you to see a document's history, as well as compare the overview of two different versions of the document. Right-click on the Puncher document and select Others > History. 100 Missler Software

107 TopSolid Design Basics Exercise 14: The PDM Purging minor revisions A purge allows you to delete the unused minor revisions of a document in order to reduce the database and simplify the project tree. We will first purge the minor revisions of the puncher. Right-click on the Puncher document. Select the Deletion menu, then Purge Minor Revisions. A new window appears prompting for the number of minor revisions to keep. Enter 1 and click on to confirm. A window indicates which actions will be performed. Click on to confirm. Where are the CAD files "physically" located? Local PDM Local PDM workspace Local vault These files are still stored in the vault. However, TopSolid has permanently deleted the major revision (A) and the minor revision (0) of the puncher. Repeat the same operations for the Plate document. Missler Software 101

108 Exercise 14: The PDM TopSolid Design Basics Life cycle Up to now, all documents you created have been given the "Design" life cycle status. We will now validate the parts for manufacturing. Right-click on the Puncher document. Select the Life Cycle (A - Design) menu, then click on Validate. Even though you only selected the Puncher assembly, TopSolid notifies us that the A revision will be validated for several files. This is normal. In fact, the other files were used to design the puncher. Validating that puncher inevitably results in validating all the parts it is made of. Click on to confirm. Where are the CAD files "physically" located? Local PDM Local PDM workspace Local vault The files are still located in the vault. However, TopSolid has validated the A revision for all documents the puncher is made of. The life cycle status of each document is shown in brackets. The next checking out for edit will generate a new major (B), minor (0) revision. 102 Missler Software

109 TopSolid Design Basics Exercise 14: The PDM References This command allows you to find a document's references and view all related documents. In our case, the Puncher assembly's references are the parts and the Punch+Pin sub-assembly it is made of. Right-click on the Puncher document and select References. A window similar to the one below automatically opens and indicates the different documents that make up the puncher, as well as their part number. Close the window. Back references This command allows you to find a document's back references. For example, you can find out if a part to be changed is used and in which assemblies. Right-click on the Plate document and select Back References. A window similar to the one below automatically opens and indicates us that the Plate A.1 part is only used in the Puncher A.1 document. Close the window. Note: You can switch to the References mode directly from the Back References window, and vice versa, by clicking either on the icon or the icon in the window. Modifying the plate We will now modify the plate by adding a Ø10mm through hole to each corner of the part. To do this, we need to apply this change to the B revision in order to keep a history. Right-click on the Plate document. Select Check Out for Edit. Open the Plate document. Make four Ø10mm through holes and position them at 12mm from the nearest edges of the face. Save the document. TopSolid automatically creates a new B.0 revision for the Plate part. Missler Software 103

110 Exercise 14: The PDM TopSolid Design Basics Taking the modification into account and validating the revision Right-click on the Plate document. Select Check In. Right-click on the Plate document. Select Life Cycle (B - Design), then click on Validate. The Plate part document has now two validated major revisions. Note: If an assembly uses a validated part and if this part is modified and contains a new validated major revision, it is necessary to manually redirect the assembly on the last major revision, if necessary. Checking the references of the puncher Right-click on the Puncher document and select References. Note that TopSolid has kept the link with the validated A.1 revision of the plate. Redirecting the last major revision of the plate on the puncher We will now manually redirect the B.0 revision of the plate on the puncher. Right-click on the Puncher document. In the Redirection menu, select Redirect References. Click on the Redirect on last button and click on to confirm. TopSolid automatically creates a new B.0 revision for the Puncher assembly. This revision then contains the validated B.0 index of the plate as a reference. Right-click on the Puncher document and select Check In. 104 Missler Software

111 TopSolid Design Basics Exercise 14: The PDM Checking references Right-click on the Puncher document and select Références. The puncher B.0 contains the plate B.0. To finish the modification, we will now validate the B.0 revision. Right-click on the Puncher document, select Life Cycle (B Design), then click on Validate. Making obsolete the A revision of the plate and the puncher We have now two validated major revisions. This configuration includes two real parts that are used or available to use. In our case, we want to keep the last validated major revisions and make the previous revisions obsolete. An obsolete revision cannot longer be used in another document. For example, an obsolete A.2 part cannot be assembled. Right-click on the major revision A of the Puncher document. Select Life Cycle (A Validated), then Make obsolete. Click on to confirm. Repeat the operation for the Plate document. You can always search for back references or references in an obsolete revision. It is also possible to make an obsolete revision valid once again by changing its life cycle status. Missler Software 105

112 Exercise 14: The PDM TopSolid Design Basics Where are the CAD files "physically" located? Local PDM Local PDM workspace Local vault Modifying the handle B.0 major revision A change of handle shape should be made. To do this, we will use a new revision of the handle. Right-click on the Handle document. Select Check Out for Edit. Open the Handle document. Remove the fillets et replace them by 2mm chamfers. Save the document. Taking the modification into account Right-click on the Handle document and select Check In. Now we want to use this new handle in another puncher. To do this, we will copy and paste the Puncher assembly. 106 Missler Software

113 TopSolid Design Basics Exercise 14: The PDM Copying and pasting the Puncher document From the Project tree, right-click on the Puncher document and select Copy. From the Project tree, right-click on the 2-PDM folder and select Paste. TopSolid creates a new document called Puncher-Copy. Rename this document Puncher 2. The two assembly documents are completely independent of each other. Right-click on the Puncher 2 document et select Check In. To change the handle in the Puncher 2 document, you can either: - modify the back references of the handle; - or, modify the references of the puncher. Redirecting the back references of the Handle document Right-click on the Handle document. In the Redirection menu, select Redirect Back References. This window allows you to select the revisions to redirect and the revision to redirect to. Redirect the A (Validated) revision to the B (Design) revision. Click on the blue arrow to go to the next stage. In the tree, select the assembly that will be impacted by the redirection of the handle revision (in our case, the Puncher 2 assembly). Click on the blue arrow to go to the next stage. This will open a window listing the documents that will be redirected. Click on to confirm. Open the Puncher 2 document and check that the handle contains the chamfers. Reuse this function to get back to the handle with the A revision for the Puncher 2 document. Missler Software 107

114 Exercise 14: The PDM TopSolid Design Basics Redirecting the references of the Puncher 2 document Right-click on the Puncher 2 document. In the Redirection menu, select Redirect References. This window allows you to identify all references of the puncher. The Original Major Revision column displays the currently used revisions and the last column Major Revision allows you to select the desired major version of the object among all available major revisions. Click on the Handle line and select B (Design) in the drop-down list for the major revision. Click on to confirm. Right-click on the Puncher 2 document and select Check In. This is not the modification we want. We will therefore delete the Puncher 2 document, as well as the B.0 revision of the handle. Deleting the Puncher 2 document Right-click on the Puncher 2 document. In the Deletion menu, click on Delete. Click on to confirm. 108 Missler Software

115 TopSolid Design Basics Exercise 14: The PDM Where are the CAD files "physically" located? Local PDM Local PDM workspace Local vault The deletion is performed locally. To ensure that the deletion will be fully taken into account, it must be checked into the vault. Right-click on the Puncher 2 document, select Check In, and then click on to confirm. Note: Checking a deleted document into the vault moves this document into the recycle bin. The recycle bin works the same way as the Windows recycle bin. Regularly empty the recycle bin by right-clicking on the recycle bin and selecting Empty Recycle Bin in the contextual menu. It is possible to restore deleted documents by right-clicking on the deleted file and selecting Restore in the contextual menu. Right-click on the Puncher 2 document. Select Purge and click on to confirm. Deleting the B revision of the handle Right-click on the revision B (Design) of the handle. Select Life Cycle (B - Design), then Delete. This operation deletes the revision but keeps in memory that this revision has already been used. For example, the B revision will appear in the file history. The new revision will be designated by C. Missler Software 109

116 Exercise 14: The PDM TopSolid Design Basics Using the PDM in Client/Server mode In this exercise, users must connect to the training PDM server. Click on the TopSolid 7 icon and select PDM > Connection. Enter the required username and password in the corresponding fields. Click on to confirm. A Chat function is available and allows you to interact with users that are connected to the PDM. Create a new project, create a new part and save the project. The other users cannot view or use this project. You have to check it into the vault to make the files available to other users. Right-click on the project name, select Check In, then click on to confirm. The project is now available to users that are connected to the PDM. Using a file already opened by another user: The assembly is checked into the vault and available for edit. The assembly is being modified by another user. 110 Missler Software

117 TopSolid Design Basics Exercise 15: Creating document templates Exercise 15: Creating document templates Concepts addressed: - Creating and declaring a new project template - Creating and declaring a new part template - Creating and declaring a new draft template This exercise teaches you how to create your own document templates. Similarly to Word with.dot files or Excel with.xlt files, TopSolid 7 allows you to start with a new part, draft or assembly using default values and associated materials. Creating a new project template Create a new project and rename it My MISSLER Template. Select Blank Template and click on to confirm. In this new project, we will create a tree structure in order to keep the same document management structure for all projects. Create the following folders: Parts Drafts Assemblies Bills of material Miscellaneous Check the project into the vault. Missler Software 111

118 Exercise 15: Creating document templates TopSolid Design Basics Declaring the new project template Right-click on the project name My MISSLER Template and select Others > Add to Templates. A window opens prompting for the position of the project template: Choose a location for the template and click on to confirm. You can browse templates via the main menu by clicking on the TopSolid 7 icon and selecting File > Templates > Open my Project Templates. This project contains the project templates: 112 Missler Software

119 TopSolid Design Basics Exercise 15: Creating document templates Creating a new part template Create a new project using the previously created project template and rename it TEST. Create a new Part document, rename it Brass Part and validate by pressing the Enter key. In the Entities tree, right-click on the Planes folder and select Show to display the three basic planes. Click on the lateral icon to put the view into perspective. In the Tools tab, select Material and Coating. In the dialog, uncheck No Material, select Copper Alloys as the material category and Brass as the material, and then click on. Then select Physical Properties, open the Mass dialog, check the Automatic box, and then click on. The prepared document should contain the following information: Save the document, then check it into the vault. Missler Software 113

120 Exercise 15: Creating document templates TopSolid Design Basics Declaring the new part template We will now declare this part template. 1. The part must be declared as a template in a specific project. Drag the Brass Part document into the project s Templates folder. Two cases are possible: 1 st case: Templates 2 nd case: Defaults When creating a new part, you can choose the template to be used among all available templates. When creating a new part, TopSolid automatically selects the default template. 2. The part must be declared as a user template. Click on the TopSolid 7 icon and select File > Templates > Open my Templates. Copy the Brass Part document and paste it into the My Templates (Documents) project. Rename the document. Check the project into the vault, then close it. Note: In this case, the part template is available at any time. 114 Missler Software

121 TopSolid Design Basics Exercise 15: Creating document templates Creating a new draft template In the same project, create a new document, choose Draft as the document type, then select Blank template. Rename the draft Your company name Draft and validate by pressing the Enter key. We will now create a draft using an A3 landscape format. Right-click in the draft s graphical area and select Format. Select the A3 ISO Landscape format in the drop-down list and click on to confirm. In the Sketch tab, select Title Block. Warning: Every time you click on this icon, TopSolid creates a new title block. The Title Block function allows you to create the main title block and auxiliary title blocks. The sketch functions are available for creating a title block, as well as cell division and text/image insertion functions. Create the following title block structure. Missler Software 115

122 Exercise 15: Creating document templates TopSolid Design Basics In the Sketch tab, use the Divide Cell function to divide the right part of the title block into four identical cells. This function allows you to create a mini-table within a cell. In our case, we want to create four rows in the right cell. Click on the right cell, set the row count to be 4 and the column count to be 1, then click on. Finish building the title block structure in order to produce the following result. 116 Missler Software

123 TopSolid Design Basics Exercise 15: Creating document templates We will now complete the title block with the necessary information. Insert a fixed (manual) text in the title block using the Text function of the Sketch tab Text writing Text positioning in the cell Text formatting Right-click on the text, select Annotation Alignment, then constrain the text with an alignment of 3mm. Missler Software 117

124 Exercise 15: Creating document templates TopSolid Design Basics Right-click on the text again, select Annotation Centering, then center the text by selecting the two vertical lines of the cell. Finish inserting the following fixed texts in the title block, then constrain them using the previous functions. Insert your company s logo using the Image function of the Sketch tab. Image size Vertically and horizontally center the image in the cell. Validate the title block edition by clicking on the button. 118 Missler Software

125 TopSolid Design Basics Exercise 15: Creating document templates You should end up with the following result: All information included in this title block is fixed. We will now insert information that will change according to: - The document properties: date, scale, author - The properties of the set to project: description, mass, material The document properties are always present and can therefore be used; these are localizable properties. However, the properties of the set to project depend on this set. To create the template, the document must include a set to project. Create a new Part document using the Steel Part template in Standard Templates - United States. Rename the document Block. In the Shape tab, create a 100x100x100mm block. Enter the following properties for the part: - Description: Block - Part number: P01_01. Save the document. In the draft template, use the Set function in the View tab, select the Block part document in the dropdown list, then click on. This operation allows you to point the set properties (description, material and part number) to the title block s cells. Right-click on the title block and edit its resolution. Missler Software 119

126 Exercise 15: Creating document templates TopSolid Design Basics Insert the text related to the document properties using the Text function. Click on the icon in front of the Text field and select Parameter from Document. In the title block, insert the Creation Date parameter which corresponds to the draft creation date. Then insert the name of the author. This parameter is available in the drop-down list of the Text field. 120 Missler Software

127 TopSolid Design Basics Exercise 15: Creating document templates The title block should contain the following information: Insert the text related to the set properties using the Text function. We will use the properties of the set to project to insert the following information in the title block: Description, Material Description, Part Number, and Major Revision. Missler Software 121

128 Exercise 15: Creating document templates TopSolid Design Basics Create four views as shown opposite (3 views + 1 perspective). Set the scale factor to 1/2. The template is now ready to be used. You just have to break the link with the Block set. In the Entities tree, edit the set to project, select <unspecified>, then click on confirm the operation. to The views and the title block must be blank when breaking the link. Save the document, then check it into the vault. 122 Missler Software