TUTORIAL ON PRO-E 2000i

Transcription

1 MIE 313 Design of mechanical components TUTORIAL ON PRO-E 2000i March 8 th Y2K - SANTOSH SHANBHAG

2 This tutorial will introduce you to a few features of Pro-E to help you get started with your project modeling. It is in no way an in depth tutorial of Pro-E. Hence if you have any specific questions do not hesitate to get it over with, during the course of this tutorial. The features that we will be going through today for the model shown are: 1. Extrusion 2. Cut 3. Blend 4. Holes 5. Chamfer. Fillet 7. Mirroring 8. Off setting 9. Engineering Drawing a) You first got to open a new file and name it as <jobname>. See to it that the radial button corresponding to PART under type and the radial button corresponding to SOLID under subtype are on. b) Secondly, it is a good procedure to set the units to the system that is desired before you go ahead with modeling. To do this Menu manager>setup>units And set the units you desire. Though these units can be changed later during or after modeling, it is a very cumbersome procedure. c) You are now ready for the modeling procedure. But before we get into this, you might want to change the default-coloring scheme. You could do this by Utilities>Colors>System Change the colors of the background, geometry etc. to suite your style. d) Let us first begin with the base. 1. Create a datum plane Menu manager>create>datum>plane>default 2. Crate the protrusion Menu manager>create>protrusion>extrude Solid Done One side>done Select DTM3 as the sketching plane>okay

3 NOTE: when One side is selected, the direction of the red arrow is the direction of extrusion. If Two Sides is selected the direction of the red arrow would be the direction of view. Sket view>right> Select DTM1 3. Create the geometry Click on intent manager (This is an easier way of creating the model, where the alignment is automatically handled by Pro-E.) Select any 2 axis to align your geometry to >Done sel Construct the geometry as shown in the figure. Set the dimensions as shown to get an accurate model. Regenerate>Done 4. Create the extrusion depth The direction of the red arrow is the direction of extrusion Set the depth = 10 e) Let us now create the shaft on top. 1. Create the protrusion and the geometry as shown in the figure following the same procedure as in the base. 2. Select the appropriate datum planes and axis for alignment.

4 f) Now create the conical portion of the shaft. 1. For this, we will be using the blend function of Pro-E. Menu manager>feature>create>solid>protrusion>blend>solid>done Parallel>Regular see>sketch sec>done Straight>Done Select the top of the cylinder created in the previous section as the sketching plane Create the bottom of the cone. Make the required changes in dimension and regenerate Sec tools>toggle. (This would grey the circle that was just created.) Go back to sketch and create the top circle and press Done Blind>Done Enter depth = and press Preview. NOTE: There might be a problem of direction of extrusion. If the extrusion occurs in the wrong direction, go to the Element Menu and double click on direction. Notice the direction of the red arrow. If this is not the desired direction of extrusion, click on flip and say Okay 2

5 g) The rest of the shaft. 1. Follow the same procedure as above for extrusion and create the rest of the shaft, the dimensions of which are shown in the figure. 2 2 h) Creating the cut Feature>Create>Cut>Solid>Done One side>done Select the plane for making the cut (sketching plane) Draw the geometry as shown Give a depth = 4

6 i) Creating the mirror image of the cut 1. For obtaining a mirror image of the cut, we will need a plane about which it should be mirrored. For this we will create a new plane offset to DTM3. Menu manager>feature>create>datum>plane>offset>plane pick DTM3 Done sel>enter Value> 5 (Notice the direction of offset. Use negative offset if required) 2. Now we can mirror the cut about this plane. Menu manager>feature>copy>select>independent>done select the cut >Done Select >Done Select the new datum plane created as the reference for mirroring. >Done j) Creating the holes 1. To create the holes Menu manager>feature>create>hole>straight>done Linear>Done Select the placement plane and give the 2 edges or planes for dimensioning. One side>done Thru next>done Enter dia = 2 2. Obtaining the other 3 holes. Use the mirror technique followed in the previous exercise. k) Chamfers and fillets. 1. Chamfers Menu manager>feature>create> Chamfer>Edge 45Xd> enter the value of d=0.25 Select the corners to apply the chamfer 2. Fillet Menu manager>feature>create> Round>Simple>Done Constant>Surface to Surface> Select the top of the base and the surface of the first extrusion from the base. Enter a radius = 0.25>Done

7 l) Making an Engineering Drawing 1. Select a new file and name it <jobname>. Do not forget to set the radial button corresponding to drawing. 2. Now a new window appears where you assign the name of the file of which the engineering drawing has to be made. Also set the size to A 3. Now create the front view Menu manager>views>add view>general>full view>noxsec>noscale Now select a point on the sheet where you want your front view to be placed. (select it nearer to the bottom left of the page). Pro-E requires you to tell it which face has to be referenced as the front face and which one as the top. So make your selections and say OK. 4. Now create the top and side views Add View>Projection>Full View>NoXsec>No Scale>Done Select a point on the sheet where you want the view to be placed. If you select to the right of the front view a side view is obtained and if you select the top of the front view, the top view is obtained. 5. To create an isometric view. Follow the same procedure as in front view, but do not set any reference front or top surfaces. Instead press the default button.. To set the dimensions Menu manager>detail>show/erase This will pull up a window using which various dimensions can be obtained. Note that these dimensions do not change the geometry. They are driven dimensions and change if the dimensions of the geometry are changed.