What do you mean by merging ? Was it just compound part creation ?
No, it was Merged in FE Model window.
If I use “Create Compound Part” in Geometry window then it wont allow me to hex mesh the individual parts of the bolt-head-nut.
This feature only assigns the elements from multiple separate parts to one common part without actually changing the mesh: Merge parts in FE models - #5 by Matej
Hex meshing on compound parts is only possible with the transfinite algorithm.
Yes, for that you would need volume partitions done in such a way that those condition are met. It’s not always feasible but often worth giving a try for simpler geometries.
if i can remember properly, single bolt is a specific case. The mesh need to be perfectly symmetric, boundary condition and loads also. When these are not fullfiled then bolt will rotate around its own axes lead to convergence problems or hard to achieves.
@synt This makes perfect sense. I did not consider the possibility of the bolt rotating about it’s own axis. I think the best alternative is to use only half the model and use symmetric BC like you have shown.
If you want to do it manually, you can use the Exploded view.
1 Like
Of course, the Exploded View 
Why did I not think of that !?
Thank you.
I made the conversion of the Ansys mesh into a PrePoMax/CalculiX mesh with the Gmsh tool. Described a bit in the following link
And with the same meshes the result comparison are looking unbelievable close.
3 Likes
Dear AsuraEquation,
I am struggling with the same problem as you with the interference fit. I am trying to use the compound part function, but it won’t let me mesh a compound part that has an interference (ie. penetration of the bush onto shaft). When I create a compound part of the bush and shaft, it actually creates 3 solid parts - one for the shaft and two for the bush. It splits the bush part into two, one which is the solid that penetrates while the other is the solid part outside the shaft. I have tried using, as Gunnar suggested, a split compound mesh too but it still fails to generate a mesh.
Please could you clarify how to use the compound part approach. I have been trying to get this to work for weeks but am completely stuck.
I’ve attached some pictures for clarity.
Kind Regards.
If you get a third part when creating a compound, your geometry does not precisely match, and the intersection of the geometry becomes a separate/third part.
You can try to fix the geometry. If the geometry is matching, then conversion to .STEP file can be the root of the problem. In this case, create a larger bushing (green part) so that the intersection volume is larger and will not cause problems while meshing. Having an additional third part will not limit your model in any way.
You don’t necessarily need compound part. You can just apply similar fine enough hex meshes to both parts. This should be sufficient for interference fit modeling. Here’s a 2D example: https://www.youtube.com/watch?v=sos-6ilPIZc
Hi PrePoMaxwell (cool nickname),
I have been experimenting with PrePoMax on contacts between cylindrical surfaces for a long time now, and I have noticed some problems.
I am preparing some material to upload in the forum to do some checking, but it will take a while because I am trying to make models that are easy to check.
I highly recommend the video FEAnalyst linked to you, which is really well done.
I recently calculated a system similar to yours so I have a few suggestions for you:
-Do not use “compound parts”;
-Set “Adjust=No” in the contacts. This often (very often) creates problems with the results being completely nonsensical. In this case you have a situation where you are obliged to put “Adjust=No” (and FEAnalyst in the video explains why), but I recommend always doing this in the cylindrical contacts.
-Also do a simplified model following the FEAnalyst video, it will come in very handy, but check that the contact pressure makes sense. If the 2D model gives you very very high values and peaks then change the mesh and use GMSH mesh.
-If even with all these measures you find strange values (very high peaks and almost zero contacts in other areas) then change the contact from ‘Hard’ to linear and change K as indicated (1/5 - 1/50 of E). You will have to do a bit of trial and error until you find a pressure similar to that calculated analytically. It sounds like a laborious and imprecise procedure, but actually comparing the data with ANSYS gives very similar values (ANSYS calculates the rigidity automatically although I haven’t figured out how yet).
1 Like
I will contribute too. I have recently validate with analitical solution an interference fit slip resistance under torsion
Yes, if the interference fit has already been modeled in the CAD this won’t work with compound. However, for the shown case I wouldn’t model it in CAD but rather after meshing, by first creating a coincident mesh and then by scaling one part in radial direction to achieve the desired interference (Model → Part → Transform → Scale). This allows to achieve quite usable results with a fairly coarse mesh.
Hi FEAnalyst, AsuraEquation, ANYS, Gunnar,
I initially followed your tutorial however the results didn’t match when I attempted to do the same in 3D.
I have since figured out the issue and have been able to get very good agreement for the 3D model.
The issue was simply that I had to enable mid-side nodes. I had selected second order mesh but when I went into the advanced settings in mesh parameters, the mid-side nodes were not enabled.
I’m not sure about my reasoning but I think once I enabled the mid-side nodes setting, it actually made the mesh second order as the mid-side nodes allows the elements to “map” a curved path when earlier it wasnt? I’m only a beginner at FEA so I’m not completely sure.
Either way, I have got it to work now.
Thank you all for your input.
Kind Regards.
Thank you all for your guidance and quick responses.