The link is not working. Please first set access to “Anyone with the link”, then copy the link and paste it here.
1 Like
I think you should be able to download it now.
Unfortunately, it’s still not working. After changing the access setting, you have to generate a new link and paste it here.
Now I can access it. The first problem I’ve noticed is this: Don't apply concentrated force load to surfaces
However, to check the connections, you should run a frequency step first. Regarding them:
- you should refine the mesh (especially on the welds) and consider using extruded hexahedral mesh wherever possible (then you could switch to linear C3D8R elements)
- you can use the Search Contact Pairs tool to generate tie constraints automatically (just check them and remove the redundant ones e.g. between the plates if not needed due to welds)
- tie constraint should have master surface on the coarser side (the automatic tool doesn’t check that)
- you may need to disable adjustment (to avoid mesh distortion) and increase position tolerance for some tie constraints
Try applying those tips in this file (I started doing it there just to show you the idea, but you should continue with mesh refinement and tie constraint corrections):
Remodeled FEA2 mod.pmx (2.7 MB)
Note that I defeatured the top part to mesh it with hex elements. If you want to keep the subfaces for load application, partition the face in CAD (e.g. FreeCAD can do it easily) instead of making shallow cutouts.
1 Like
Thanks very much, for working on this file, I’m trying to see how I can move forward by editing based on your recommendations. for the subfaces, I need to apply loads on those area, as the part which apply force is connected through those surface, I tried to import the model with just a sketch but it wasn’t visible in the step format and the only way I found to be able to have them in my model was having shallow cut, or making separate surface in the CAD. with the Surface I tried in different model and noticed those surface are being recognized as separate part, if you have any other recommendations on that, I would be happy to hear.
Thanks
You could keep those patches as surface partitions. Easy to do (after removing the shallow cutout) in FreeCAD with a sketch and Boolean fragments tool. As a result, you get this:
Remodeled FEA2 face partitions.zip (7.1 KB)
And you can generate hex-dominated mesh while still having the surfaces for load application:
hi i have modelled two parts one is running but the other model is not running but the contact conditions are same for both the models. can you please help
Column bolt model is running properly
11.3.2025.pmx (5.8 MB)
column bolt.pmx (2.2 MB)
Try this:
11.3.2025 mod.pmx (1.8 MB)
@FEAnalyst I prepared the model with the old version 2.3.0 and the model runs i got the results , but in the new version the it is failing says “non Jacobean”
What i modified this time is side face bolt contact adjustment to 2.0mm as the gap between the bolt and plate hole face is 2mm so it is running in old version but it fails in new version.
11.3.2025 new version 2.5.0.pmx (3.2 MB)
11.3.2025 old version 2.3.0.pmx (1.5 MB)
Whenever you get negative jacobian errors, you should always check if you have adjustment enabled in tie constraints or contact pairs and disable it. Here, disable it in the third contact pair.
11.3.2025 new version 2.5.0 mod.pmx (1.8 MB)
I’m using SolidWorks as CAD software, I tried to generate STEP file with sketches but they didn’t show up, I also tried to mount the attached part, you’ve shared but the sketches weren’t visible in STEP format after making assembly and generating STEP. I have a doubt I’m able to generate sketches in SolidWorks, probably I should use Free Cad. Or if you have any suggestions in SolidWorks I’d be happy to know.
Thanks
Or is there any way to draw the curves in PrePomax?
You can’t do this kind of a partition in PrePoMax (only splitting by two points is possible). And you can’t import sketches to it or create curves there either.
So you have to do it in any CAD software - partition the solid model, then export it to STEP (without the sketch itself) and import to PrePoMax. Previously, I shared with you such a file obtained in FreeCAD, but you can definitely do it in SolidWorks too. I think that you need the Split Line tool there: https://www.youtube.com/watch?v=yFzMqYlTxsk
There is no issue with making the the required pattern on part, I’ve made it with split line in SolidWorks, the problem is with exporting it to STEP with SolidWorks, the (Split line) won’t be exported to STEP. During my research the only way is making shallow cut extruding or exporting in Parasolid, which is not supported in PrePomax.
I’m not sure about SolidWorks, I haven’t used it for years. I thought that applying Split Line and then exporting the geometry to STEP would suffice (the model would be imported without the tool curve but with an additional subsurface). That’s how it works in FreeCAD - you apply Boolean fragments and export this object to STEP. This gives you the geometry like the one I shared yesterday.
It seems like the problem is with SolidWorks exporting, I’m trying to make new assembly with Free Cad, and at the same time apply mentioned changes in PrePomax on the first modified model you shared with me, is this a bug that I’m not able to see mesh refinement? in the geometry tab there is only the mesh parameters.
What version of PrePoMax are you using ? Mesh refinement was renamed to Local Mesh Size in v2.5.0.
I’m using v 2.5.0 and you’re right it’s local Mesh, Thanks very much.
Hi
I have applied your suggestions and got these results. I was expected to have more stress on wildings. I may missed some functions. I have also attached the link. If there is an similar model that I can take a look at it as a reference it would be great help, it’s my first FEA in PrePomax and I am trying to have some studies beside.
