How to model Support Bracket in Inventor 2011?

In this tutorial we will model a support bracket, add welds and do a simple FEA test.
The modeling was in Inventor 2011 but the same commads can be used in Inventor 2012 and 2010.

  1. Step 1:

    First we create a new part file. I will be using mm units.

  2. Step 2:

    We create a rectangle using the rectangle command using the dimensions shown in the next image.

  3. Step 3:

    Next we constraint our rectangle to the center of our work plane. First vertically

  4. Step 4:

    And then Horizontaly. It is very important to do so in all our parts. When we are finished we click Finish Sketch.

  5. Step 5:

    We choose the extrude command and select the sketch we drew (it should be autoselected). We use 10mm as an extrusion value and click OK.

  6. Step 6:

    Then we select the top face. Three icons appear. We click on the far right wich is for creating a new sketch

  7. Step 7:

    Using the point command we place four points on the face. Using the constraint commands (steps 3 and 4) we constraint the points vertically and horizontally

  8. Step 8:

    Using the dimension command we add the dimensions shown and then click finish sketch

  9. Step 9:

    We use the hole command and a new window appears. Our points should be autoselected for hole centers. If not select them manually. In the window we choose 14mm for our holes diameter and through all for termination. Then we click OK.

  10. Step 10:

    Finally we will add properties to our part. In the model browser right click Part one and in the menu choose iProperties.

  11. Step 11:

    Go to Physical tab and in the Material drop down menu choose Steel Mild. We will need those properties for our FEA test. Once you are finished save your part.

  12. Step 12:

    Create a new part with the dimension shown in the image using the exact same steps as above. The holes should be in the center of the part. Add properties and save.

  13. Step 13:

    Create a new part with the dimension shown in the image using the exact same steps as above. Add properties and save.

  14. Step 14:

    Choose new and choose Weldment (ISO).iam

  15. Step 15:

    In the Assemble tab choose place component. In the new window browse to the location we saved our first part, select it and place it. By deafault the first part that is placed in an assembly or weldment file is grounded. You can change that later but for this tutorial we will keep this configuration.

  16. Step 16:

    Do the same for the second part.

  17. Step 17:

    Using the constraint command and selecting Mate we choose the faces of our parts shown in the red arrows. then select Apply.

  18. Step 18:

    This is what we should be looking at if everything was done correct.

  19. Step 19:

    Then choose flush instead of mate (red circle) and select the two faces shown. In the Offset value (red circle) put 40mm offset. Click Apply.

  20. Step 20:

    Expand Part1 and Part 2 in the model browser. With the flush command still active choose the YZ plane of part 1 and YZ plane of part 2. Click OK.

  21. Step 21:

    This is what we should be looking at. Now Part 2 is fully constraint.

  22. Step 22:

    Next we place our third part 2 times. Use the exact same steps for placing part 2.

  23. Step 23:

    Click on Constrain command and using Mate select the face of part 1 and the face of part 3 as shown. Do the same again for the second instance of part 3.

  24. Step 24:

    Our model looks like this.

  25. Step 25:

    Using the flush constraint choose the two faces shown in the circles. Click Apply.

  26. Step 26:

    Then use the mate constraint and choose the face of part 3 and the face of part 2. click Apply.
    Still part 3 is not fully constraint.

  27. Step 27:

    With the mate constraint still active select the face shown here...

  28. Step 28:

    ...and the face shown here. Use 110mm for an Offset value and click apply.

  29. Step 29:

    Using the Flush constraint select the face of part 3 and Origin's YZ plane from the model browser (as shown in red circle). Click OK. Now our model is fully constraint.

  30. Step 30:

    Go to Welds tab and click on Welds->Fillet

  31. Step 31:

    A new window appears. In this window we will put our weld values.

  32. Step 32:

    With 1st face selected choose the blue face. then go to the weld window choose 2nd face and select the green face. A preview appears on our model.
    Use 5X5 as input values for weld heights.

  33. Step 33:

    In the Intermittency use the values shown in the image and use 20mm as the first offset value. This will create 3X20mm long, 5mm high welds with 40mm spacing. Click Apply.

  34. Step 34:

    Do the same in all sides

  35. Step 35:

    For this side just erase the values in Offset and Intermittency and choose the appropriate faces. Click Apply.

  36. Step 36:

    Next select the faces shown in blue of part 2 as a 1st selection...

  37. Step 37:

    And as a 2nd selection the face of part 1 in green. Click Apply.

  38. Step 38:

    Do the same in this side ou the assembly.

  39. Step 39:

    Once finished click return and save the assembly.

  40. Step 40:

    Go to enviroments and choose Stress analysis

  41. Step 41:

    Choose create simulation and click OK

  42. Step 42:

    Now we should add costraints. Choose fixed constraint.

  43. Step 43:

    Choose the holes in part 1 and click OK.

  44. Step 44:

    We will now add a force. Go to Loads and click force.

  45. Step 45:

    Select the top face of part 2 and give a 300Newton value. If the force is upside down use the diretion button in the force input window.

  46. Step 46:

    Change the mesh settings using the values shown

  47. Step 47:

    Select Mesh view. After a while our model looks like this.

  48. Step 48:

    Click Simulate and a new window appears. Click Run. After the calculations are complete we have our model in this state.

  49. Step 49:

    We can change the display settings, the displayed values, add probes export reperts and animate the results.