Starting a New Drawing with a Title Block and Border From the File menu select New. Within the New file menu toggle the option Drawing, name the file and turn Off the toggle Use Default Template. Select OK In the New Drawing dialogue: Specify the Default Model. This is the file from which the drawing views will be extracted. It can be a model or an assembly file. The file need not be open to use as the default file. To search for a specific file, select Browse. Toggle the option Empty with format For the Format select Browse.
This opens a file dialogue window. Search the folder System Formats. Choose the format based upon the desired paper size. Paper Sizes: (values in inches) A 8.5 x 11 B 11 x 17 C 17 x 22 D 22 x 34 E 34 x 44 This will open a new drawing file with a titleblock and border included. Appearance will be similar to the figure at right.
Set the file options: In the Drawing menu, select Advanced and Draw Setup. The Options window will open. Change to following settings: Set draw_text_height to a value of.125 To do this, pick the option from the list, enter the new value in the window at the bottom and select Add. Set draw_arrow_length to.125 and set draw_arrow_style to Open. When finished select OK and the changes will be made to the current file. In addition, all new drawings created during this session will have these settings.
To Add Views to a Drawing From the Drawing menu, select Views > Add View View Type Settings For the first view added to a drawing select View Type > General (Note: this can also be used to add an isometric view to an existing drawing) Other view types permit the creation of projected views. Projection: Create an Orthographic projection from an existing view. Auxiliary: Create an Auxiliary projection from an existing view. Detailed: Create a scaled view which depicts a specified portion of an existing view. Use this option to create a view which so a detail of existing view magnified. Revolved: Create a revolved section Full View: Show a conventional view Half View: Show a half view; used with symmetrical parts Broken View: Show object with a conventional break; used for long narrow objects. Partial View: Show a portion of a view delimited with a jagged boundary Scale: User will specify a scale value for the view No Scale: Software will determine a scale value based upon paper size and object dimensions. Section: View will be shown in cross-section No Xsec: View will not be shown in cross-section Our first view will use the default settings of General > Full View > No Xsec along with the non-default setting of Scale. You are prompted to specify the center point for view. Simply pick a location on the screen. The view can be moved later. The view will be inserted in default orientation.
The next step is to orient your general view. This process is similar to orienting your sketch plane when creating a feature. You choose will choosing two planar features (either surfaces or datum planes) to serve as references. Each reference will have a facing direction (Front, Top, Bottom, Left, Right) For example choose a feature for Reference 1 and specify it to face Front (facing is the outward normal vector for a surface and the yellow side vector for a datum plane). Choose a feature perpendicular to Reference 1 and specify it to face Top, Bottom, Left or Right. If you make a mistake, the Default button will return your orientation to default and then you can start over. Adding Projected Views To add a projected view to a drawing, select: Add View > Projection > No Xsec > No Scale > Done You will be prompted to select the Center Point for the view. The position you select, with respect to the existing view, will determine the projection that is created. For example, pick to the right to get a right-side view. Our example shows a front view created below a top view.
Preparing for a Section View by Creating an X-Section in Part Mode First create an X-Section (this is Pro/E s term for cross-section ) in the part file from which the drawing views are extracted. This creation can also be done in Drawing mode but I think it is easiest to learn this way. In the Part menu select X-section and then Create All sections are either planar or offset. You will probably create more planar sections than anything else. Select Planar > Single and Done. Enter a name for the section. This name will appear when the section is placed in a drawing. For example, a sections named A will be labeled Section A A. Select a planar surface or a datum plane to define the section. The section will be displayed within the file. Select Done to complete creation. If you do not wish to display the section in the part file, use the X-section command Erase and select the section from the displayed list of names.
Creating a Projected View in Section in Drawing Mode: Begin as you did for the conventional projected view except set the toggle for Section. Add View > Projection > Section > Scale > Done Next set the section properties. Sections can be Full, Half or Local. A local section is the term used for a broken-out section. Examples of Half and Local sections are given later in this document Select between Total and Area cross-section. A Total cross-section shows all features beyond the cutting plane as visible and an Area cross-section shows only the material cut by the cutting plane. Next you are prompted to select the Center Point for the view. Select a cross-section to retrieve. If you have already created an X- section as detailed above, the name will appear in the list. If you have not created the X-section yet, it can be done in Drawing mode. Choose Create from the menu and follow the same procedure as you would in Part mode. Pick a view for the arrows where the section is perp, This somewhat obtuse statement is asking you to select the view where the cutting plane line will be placed. To move the section label, simply pick to highlight, then drag.
To edit the crosshatching appearance (angle, spacing, linetype), pick the hatching to highlight, then press the RMB to open the edit menu. Modify Spacing Menu Modify Angle Menu Half Sections When Half Section is specified, the user is prompted to select the reference plane for half-section creation. This is the plane that delimits the extents of the half section. Typically a datum plane is used. Arrows will be displayed. These are pointing toward the half of the view that will appear in section. Note: this is NOT the cutting plane line that will appear for the section. The direction may be flipped. Note that the Disp_Mode of the view was modified to remove hidden lines.
Local Sections Pro/ENGINEER uses the term local section to refer to a broken-out section. When Local Section is specified, the user is prompted to select the center point for section breakout area. This is a point within the area to be broken out. Next the user is prompted to sketch a spline to define the outline of the break-out. Begin picking points off the object, then move through where you would like the break line. Press the MMB to end point input. Creating an Auxiliary View Select Views > Add View > Auxiliary Set other options as desired (full vs. partial, section vs. no section). Select Center Point for view. Prompt says; Select edge of, or axis through, or datum plane as, front surface on main view. This prompt is asking you to select the feature to project perpendicular to. For a primary auxiliary this typically means the line view of an inclined surface.
Creating a Detailed View Select Views > Add View > Detailed There are no options with the Detailed view format. Select Center Point for view. Enter View Scale Detailed views are typically scaled larger to show some small detail of the component more clearly. Prompt says; Select Center Point for detail on an existing view. This is asking you to select the center of the area on an existing view that your would like to magnify and display in the detailed view. The point must be a node of an existing entity, such as a line endpoint. It is not critical for this point to be at the exact center of the area you want. Sketch a spline, without intersecting other splines (such as from a partial view or local section), to define an outline. Press the MMB to end spline input. Enter a name for the detailed view. Next, from the open menu, select the shape of the boundary that will delimit the area on the existing view from which the detail has been taken. Select location for Note. This is the note that will reference the shape defined in the previous step, and which specifies to See Detail (detail name here).
Creating a Revolved Section View This view will require creation of a X-section, either prior to creating the view in Part mode or on the fly during the view creation command. See the previous portions of this document covering Section Views for reference. The view is actually not created in a line of projection perpendicular to the section cutting plane. This may be non-intuitive. It may be helpful to examine the example below and then to read the instructions. Select Views > Add View > Revolved Set other the option as desired (full vs. partial). Select Center Point for view Select a parent view for the revolved section Select a cross-section to retrieve by picking a name from the menu. The view is not labeled. The center indicates where the view is taken. The centerline can be changed in length or erased. Other View Commands To Move a View Pick the view, a border will appear around the view and you will be able to drag it to a new location. Pick with the LMB to set the new location. If the view has associated children (view which were created as projections from it), they will be moved also.
Erase View This command will remove a view from active display. A green box labeled with the view name with will replace the erased view. The view still exists and may be displayed again through the Resume View command. Delete View This command will remove an existing view from the drawing file. Child views of the deleted view, must also be deleted. Modify View Opens a menu with several options. Choose the option and then select a view. These options include: View Type: Select view and you can change view type. For example, Project to Auxiliary. Change Scale: Change the scale setting for a view created with the Scale option set. View name: Change the name of a named view, for example a Detailed View. Reorient: Change the view s orientation. Child views will be affected. Alignment: Allows the user to over ride the default alignment settings of views. For example, to move a Projected View out of line-of-projection. X-Section: Allows the user to change which section is retrieved and displayed in a view that includes a section. Add Arrows: Use to add a cutting plane line to a section view. Del Arrows: Use to remove a cutting plane line from a view.
Disp Mode: This command is used to change the default display setting for a view or for individual edges. This is often used to remove Tangent Curves from display. Tangent Curves are the face boundaries of fillet and round entities. They are not display in mechanical drawing and hence, their display must be suppressed. The sample views shown depict a cast part. As a cast part, it includes fillets and rounds. In this case, the Display Mode setting for the views should be changed. View Display: This option changes the display of certain line types (such as Tangent Edges) for an entire view. The top portion of the View Disp menu allows the user to set the view setting for hidden lines. The default setting refers to the icon setting at the top of the screen. Note: If the default display setting is set to Shade, you will be unable to alter the display of hidden edges. The center portion of the menu allows the user to change the display setting for Tangent Curves. If we set the option to No Disp Tan and select the top view in our example, view display will appear as shown.
In some cases the algorithms used to determine which edges to remove using the View Disp option will not remove all the desired edges or will remove edges which should still be displayed (see examples). In these case, the user should use the Edge Disp option to remove individual edges. The Erase Line should be chosen and the individual edges to be removed should be selected in the drawing view. Selected Edges Final View