How to make and assembly a Pillow Block using Solid Edge


This is part 1 of my tutorial where I will try to explain how to model the base of the pillow block. Resuming I will show you how to:
- Define where you want to do your sketch using coincident or parallel planes
- Will see how to draw geometries and how to dimension and use geometric relations
- Create features using Extruded, Extruded-Cut, Revolve, Revolve-Cut and MIrror
- Make a thread hole.

  1. Step 1:

    When you open Solid Edge you will see the following window (figure 1). As it is intuitive click in “ISO PART” to model a new piece.

  2. Step 2:

    Now depending of the software version you are using the commands can be disposed in a different way although the concept will be the same. For those who are beginning with Solid Edge I think that Synchronous Technology show be discussed later, so we will model our parts using the “traditional way”. I mean we will do 2D Sketches and then using features like Extrusions, Revolves and others will generate our pieces. By standard Solid Edge ST4 sets automatically Synchronous Technology on, so to disable it go to Tools tab and check “ordered”. See image in case of any doubt

  3. Step 3:

    Return to “Home” tab and click on “Sketch” command. As you can in the bottom of the screen you have “Prompt Bar” saying to choose a plane to begin drawing. Note also that after you clicked at Sketch a new bar appeared. This bar is very important as it is where you choose which plane you want to use. You can choose to draw in a coincident plane or for example in a parallel plane at a specific distance from the reference plane. In our very beginning we will use a plane coincident to the default plane to sketch (Front XZ). To do this in the features tree expand “Base reference planes” and click left click in “Front XZ”.

  4. Step 4:

    Now it’s time to create our geometry. Choose “Rectangle by center” and draw a rectangle centered with the Origin. You should get something similar to the image below.

  5. Step 5:

    Now in the “Home” tab choose Smart Dimension and next select the bottom edge of you rectangle. Than drag the dimension to good place, left click and digit the dimension in the window that appeared (255 mm).

  6. Step 6:

    Repeat step 5 and put width with 28 mm

  7. Step 7:

    Now we will draw a “Circle by center point”. Move your mouse to the origin and then move it up. Notice that the vertical alignment line extending from the cursor snaps into position and is displayed dashed when the cursor is vertically aligned to the origin point. This is a very helpful tip! Now left click and create the circle, than using Smart Dimension put 100 mm of diameter.

  8. Step 8:

    Using Smart Dimension left click on the bottom edge of the rectangle and in the circle than give it 70 mm.

  9. Step 9:

    Draw a new circle concentric to the first with 125 mm of diameter. If you pass with you mouse over the first circle and then go to the origin you will notice that automatically will appear an icon coupled to the mouse representing concentricity and you just need to left click.

  10. Step 10:

    At this point I think you have capability to draw the remaining lines. So draw and dimension the remaining lines as exposed in the next image:

  11. Step 11:

    We will need to trim some lines in order to reach our pretended geometry. See image to find the correct command to trim and then left click on the lines not needed to eliminate them.

  12. Step 12:

    We have completed our main geometry and now we will generate our 3D Solid. To do this begin by exit the Sketch (this command is in Home Tab on the right side). Now select Extrusion Command (in Home tab). A new bar will appear and as we had already drawn our sketch, in the drop-down box we should put “Select From Sketch”, then we select our contour and finally click in the green arrow.

  13. Step 13:

    Now a new bar appear in the same position and we just need to indicate the extrusion depth which is 70 mm and that we want a symmetric extrusion to the sketch plane (See image to clarify this question) . Than give an enter and click finish!

  14. Step 14:

    Create a new Sketch with the following contour (see image). Than exit the sketch and extrude the contour symmetric to the sketch plane and put in depth 95 mm.

  15. Step 15:

    Create a new Sketch coincident to the top base face, draw and dimension the following geometry (see image). Draw also a vertical line at the middle. This line will be used for mirror our geometry.

  16. Step 16:

    Let’s learn how to mirror elements. In the draw section (Home Tab) you will find mirro command. Left click on it. As you click in the prompt bard will tell you to select those elements you want to mirror. As we will select multiple elements, press Ctrl and select all the elements that compose our geometry. Than release control and a new task will appear in the prompt bar. In this case we should select the line to mirror about which is the mentioned in STEP15. See the following image to see the result:.

  17. Step 17:

    It’s time to use the “Cut Extrude” command. This command is very similar to the “Extrude” although as it indicates it removes material. We will not specify any depth of cut. I will introduce you a new “condition end”. We will say to the software to cut until reach the bottom face of our base (using “trough next” button). To do this task check image. I am jumping some steps as they are equal to the extrude command.

  18. Step 18:

    Again, start a new Sketch but this time at top face of the part. Than draw the geometry (see image) and don’t forget to use “Mirror” command as it potentially allows you to speed up your task.

  19. Step 19:

    Exit the sketch and left click on “Revolve Command”. In Revolve Command you should do the following steps: first you choose the closed contour to revolve, next you identify the revolution axis, than you indicate the revolution axis (in this case 180o) and finally the direction to revolve. I choose not to describe this step in depth as I think that I should only give you some lights and then let you explore, but if you have any question in any of the steps feel free to ask me!

  20. Step 20:

    At this point part should look like this (see image):

  21. Step 21:

    Start a new sketch in same plane as our last and design the following geometry:

  22. Step 22:

    Exit the sketch and left click “Revolved Cut”. Again select the two contours, use the vertical line drawn in the sketch as axis of revolution, define revolution angle as 180o and select the correct direction. Here is the result:

  23. Step 23:

    Now aplly “Round command” to the following edge define radius of 2 mm.

  24. Step 24:

    Apply “Chanfer command” with a setback of 2 mm in the following edges:

  25. Step 25:

    Now start a new “Sketch” but this time we will draw in a plane parallel to the Right Plane (YZ) at a distance of 70 mm. To do this, see image:

  26. Step 26:

    Draw the following geometry (see image) and to assure that our rectangle is centred with the middle line we apply a Symmetric relation. To do this, left click on the command (you can find it at the “Home Tab” in the “Relate” section, select the two vertical lines and next select the symmetric axis, which is the middle line.

  27. Step 27:

    Extrude the last Sketch and use “Trough Next” as your condition end, this will assure that the extrusions stops exactly when it reach the cylindrical face. If you don’t remember how to set this type of “condition end” read and see image of step 17.

  28. Step 28:

    We should mirror the last feature that we had created. Left click in “Mirror” command, than as you can see in the prompt bar, Solid Edge asks you to choose which feature you want to mirror. To do this, in the tree just left click in the last feature created. Next we just need to indicate that we want to mirror about Right Plane using again the tree to select it. Finally “hit” the “finish” button.

  29. Step 29:

    And we’re almost done! Start more a time a new sketch in the top face of our solid part and draw the following geometry:

  30. Step 30:

    STEP30 – Use Cut Extrude command to make this two holes and put in depth 20 mm.

  31. Step 31:

    We did two holes of 8.5 mm because we want to thread a M10 hole. So, when you want to obtain a thread, you should create a hole with the diameter of the drill instead of a hole with the nominal diameter of the thread which in this case is 10 mm. Select “Thread” command and follow the prompt bar which will ask you to do some tasks to identify the hole to thread. After you identify the hole automatically will be recognized that you want to made a M10 with a step of 1.5 mm as you can see in the image

  32. Step 32:

    Repeat same procedure as described in STEP31 but for the other hole and we are done!


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