Shaft in hole + Contacts

[autodesk428JLG]

Hi everyone,

If i have a shaft in a hole, like with tolerance of H7 so lets say the hole is 50.03 mm and shaft 50 mm. If i want to have a reasonable approximation of what happens when loads are applied to the shaft, what kind of contacts should i use? As of now i use separation and 3D elements. The shaft doesnt rotate so i think it will just make contact and stay at the contacted location. The shaft is allowed to move in its axial direction.

Using Autodesk Nastran 2023

Best regards,

Daniel

[John_Holtz · Accepted solution]

Hi Daniel,

In my opinion, it is not possible to have a "reasonable approximation" with a gap of 0.015 mm on the radius. To preserve a gap that small would require a mesh size close to 0. (Actually, I just calculated it. A mesh size of 1 mm gives a clearance of 0.01 mm or better. A mesh size of 0.5 mm gives a clearance of 0.0137 mm or better.) The reason can be seen in this exaggerated example. The distance "across the corners" for the ID will be 50 mm, but the distance "across the flats" for the OD will be smaller than 50.03 mm depending on the mesh size.

Figure 1: Ideal bodies shown by solid outlines with the theoretical gap shaded in gray. A coarse mesh converts the cylinder and holes to squares (shown by the dashed lines). Note how the inner body interferes with the outer body depending on how the "random" nodes are positioned.

If you are trying to calculate something like the Hertz contact stress, then you only need the 1 mm or 0.5 mm mesh on a small area, and that may be feasible. (For Hertz contact stress, the mesh size should be based on the size of the contact area. You will want a few elements over the width of the theoretical contact area.)

Sorry for the diversion. The answer to your question is separation contact is correct. I think the gap can be "ignored" for most purposes, meaning the difference between a gap of 0 and a gap of 0.03 mm is negligible in most simulations unless you make the mesh very small to account for the size of the gap. The solver removes the interferences mathematically, so the analysis ends up with a 0 gap clearance.

You will need to use constraints and/or "Connectors > Springs" to prevent the part from moving freely in the axial direction and rotation. (I assume you are using either linear static or nonlinear static. Any type of static analysis requires all the parts to be statically stable; otherwise, you get an E5000, E5001, or E5004 error.)

John

[autodesk428JLG]

Thanks alot John, appreciate it alot!

Best regards,
D