# Mesh generation error **URL:** \ **Category:** General Questions\ **Created:** [September 9, 2026, 4:12pm UTC](https://prepomax.discourse.group/t/mesh-generation-error/3660 "2026-09-09T16:12:10Z")\ **Posts on this page:** 14\ **Page:** 1
**Author:** ![Agazzotti](https://avatars.discourse-cdn.com/v4/letter/a/3da27b/32.png) [@Agazzotti](https://prepomax.discourse.group/u/Agazzotti)\ **Post date:** [September 9, 2026, 4:12pm UTC](https://prepomax.discourse.group/t/mesh-generation-error/3660/1 "2026-09-09T16:12:10Z")
The mesh is not being generated for the attached model, and I don’t understand why. I created a compound part to ensure the meshes making up the model are conformal. Thanks in advance to everyone for the help. A. [Controsf\_2.pmx](https://prepomax.discourse.group/uploads/short-url/6FybZQcGKhvEUr7lkJENngtLDtA.pmx) (1.5 MB) ---
**Author:** ![SergioP1975](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/sergiop1975/32/37_2.png) [@SergioP1975](https://prepomax.discourse.group/u/SergioP1975)\ **Post date:** [September 9, 2026, 4:43pm UTC](https://prepomax.discourse.group/t/mesh-generation-error/3660/2 "2026-09-09T16:43:48Z")
I would convert the CAD model to surfaces and then create an extrude mesh from shell in Prepomax. ---
**Author:** ![FEAnalyst](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/feanalyst/32/688_2.png) [@FEAnalyst](https://prepomax.discourse.group/u/FEAnalyst)\ **Post date:** [September 9, 2026, 4:46pm UTC](https://prepomax.discourse.group/t/mesh-generation-error/3660/3 "2026-09-09T16:46:17Z")
Can you share the geometry in .step format or at least some screenshots ? I can’t open your file in the version of PrePoMax I have now. ---
**Author:** ![FEAnalyst](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/feanalyst/32/688_2.png) [@FEAnalyst](https://prepomax.discourse.group/u/FEAnalyst)\ **Post date:** [September 9, 2026, 4:47pm UTC](https://prepomax.discourse.group/t/mesh-generation-error/3660/4 "2026-09-09T16:47:30Z")
Generally speaking, see this page (especially the sections about geometry type selection and simplification/defeaturing): [https://wiki.freecad.org/FEM\_Geometry\_Preparation\_and\_Meshing](https://wiki.freecad.org/FEM_Geometry_Preparation_and_Meshing) ---
**Author:** ![FEAnalyst](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/feanalyst/32/688_2.png) [@FEAnalyst](https://prepomax.discourse.group/u/FEAnalyst)\ **Post date:** [September 9, 2026, 6:53pm UTC](https://prepomax.discourse.group/t/mesh-generation-error/3660/5 "2026-09-09T18:53:32Z")
Nevermind, got it. And yeah, definitely shells or Thicken Shell Mesh on surface geometry. ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/1/16beffed318ee21effb7ca9de6d06a9853b467a0.jpeg) Here’s an example (just a coarse mesh to show the workflow): ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/8/8de4192cdcca79744fc0bbe64a97fd56cb8b8312.png) ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/0/0925e8143d8c1ca2582af317b866e94878766340.png) ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/9/9d0ec85f779009afd44ad667f78b9d1ac30b3edc.jpeg) ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/b/b64a7231d6e93d3939975b2cfa609596c6f16e35.jpeg) [Controsf\_2\_shell.pmx](https://prepomax.discourse.group/uploads/short-url/ools3Ym3kvqdAReVRShhNJnevc7.pmx) (62.7 KB) If you want, I can show you how to do it in FreeCAD. ---
**Author:** ![MisiaKu](https://avatars.discourse-cdn.com/v4/letter/m/e5b9ba/32.png) [@MisiaKu](https://prepomax.discourse.group/u/MisiaKu)\ **Post date:** [September 11, 2026, 12:58pm UTC](https://prepomax.discourse.group/t/mesh-generation-error/3660/6 "2026-09-11T12:58:20Z")
The components are large and thin. Consequently, the mesher attempts to create a very fine subdivision. Additionally, the holes complicate the meshing process, resulting in a very high number of nodes. Perhaps the model needs some simplification? ---
**Author:** ![FEAnalyst](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/feanalyst/32/688_2.png) [@FEAnalyst](https://prepomax.discourse.group/u/FEAnalyst)\ **Post date:** [September 11, 2026, 1:04pm UTC](https://prepomax.discourse.group/t/mesh-generation-error/3660/7 "2026-09-11T13:04:12Z")
That’s why we already proposed shell or Thicken Shell Mesh approach. Meshing with tetrahedrons doesn’t make much sense here. But let’s wait for the OPs feedback. ---
**Author:** ![MisiaKu](https://avatars.discourse-cdn.com/v4/letter/m/e5b9ba/32.png) [@MisiaKu](https://prepomax.discourse.group/u/MisiaKu)\ **Post date:** [September 11, 2026, 1:47pm UTC](https://prepomax.discourse.group/t/mesh-generation-error/3660/8 "2026-09-11T13:47:05Z")
![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/f/f531b8231c1a16331d50316dee77e44c52a69f56.png) ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/a/af43651d9ebd8748c1ef6acafb5bc241ead10c45.png) ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/a/a89f7104b9b146d320353dc8d02f875dafa1607f.jpeg) Cutting errors? ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/d/d2b8f5bc617a54d1e5c15c1028494b45945c0bfa.png) ---
**Author:** ![FEAnalyst](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/feanalyst/32/688_2.png) [@FEAnalyst](https://prepomax.discourse.group/u/FEAnalyst)\ **Post date:** [September 11, 2026, 1:56pm UTC](https://prepomax.discourse.group/t/mesh-generation-error/3660/9 "2026-09-11T13:56:41Z")
It all needs to be converted to surfaces first anyway. Like I did with one of the parts, as shared above. I skipped the plates and small pins since they seem irrelevant for now. Of course, converting to surfaces/shells may involve some simplifications - see the thicker ends of the profiles. ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/a/a1b7c15772863fa823ce9b7c31d79918406bc3a1.png) ---
**Author:** ![MisiaKu](https://avatars.discourse-cdn.com/v4/letter/m/e5b9ba/32.png) [@MisiaKu](https://prepomax.discourse.group/u/MisiaKu)\ **Post date:** [September 11, 2026, 4:01pm UTC](https://prepomax.discourse.group/t/mesh-generation-error/3660/10 "2026-09-11T16:01:32Z")
Rigid Body + Nlgeom + shells = no convergence? Has anything changed? ---
**Author:** ![FEAnalyst](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/feanalyst/32/688_2.png) [@FEAnalyst](https://prepomax.discourse.group/u/FEAnalyst)\ **Post date:** [September 11, 2026, 4:10pm UTC](https://prepomax.discourse.group/t/mesh-generation-error/3660/11 "2026-09-11T16:10:41Z")
No, we discuss it here regularly. CalculiX 2.23 doesn’t allow such a combination at all, in other versions it works fine in linear analyses, but may fail in nonlinear ones. However, there was no mentioned of rigid body constraints here yet, from what I see. ---
**Author:** ![Agazzotti](https://avatars.discourse-cdn.com/v4/letter/a/3da27b/32.png) [@Agazzotti](https://prepomax.discourse.group/u/Agazzotti)\ **Post date:** [September 15, 2026, 3:57pm UTC](https://prepomax.discourse.group/t/mesh-generation-error/3660/12 "2026-09-15T15:57:44Z")
Hi, Apologies for the late reply. I managed to generate the mesh starting from shell elements. I was unable to create the bolted connection between the profiles (using solid elements) because the shell and solid meshes are non-congruent, and it is not possible to create a compound part combining shells and solids. In Ansys, it is possible to create a connection between the edges of adjacent holes, but this cannot be done in PrePoMax. I am attaching the model I analyzed (without the hole-edge connection); however, the calculation did not finish after 3 hours, so I stopped it. Simplifying the model is not an option, as it is necessary to verify the flexural-torsional instability of the coupled profiles. I would like to know how I can obtain the verification results for the model. Thanks for the help. > **[Mesh generation error](https://wetransfer.com/downloads/03fbf66885afce2eda51b165f0cca40d20260915155534/7a756c?t_exp=1789746934&t_lsid=36053eba-a9c6-4c13-9f1e-2f9dc179e285&t_network=link&t_rid=Z29vZ2xlLW9hdXRoMnwxMTY3ODU1OTkwMzYwNzE4OTAwMTQ=&t_s=download_link&t_ts=1789487759)** > > 1 file sent via WeTransfer, the simplest way to send your files around the world ---
**Author:** ![FEAnalyst](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/feanalyst/32/688_2.png) [@FEAnalyst](https://prepomax.discourse.group/u/FEAnalyst)\ **Post date:** [September 15, 2026, 4:15pm UTC](https://prepomax.discourse.group/t/mesh-generation-error/3660/13 "2026-09-15T16:15:34Z")
> [@Agazzotti](#): > > In Ansys, it is possible to create a connection between the edges of adjacent holes, but this cannot be done in PrePoMax. There are other simplified ways to model bolts. For example, you could connect holes on both sides with a rigid body constraint. > [@Agazzotti](#): > > the calculation did not finish after 3 hours, so I stopped it Try with a coarser mesh (e.g. less layers) first. Also, switch to C3D8R instead of C3D8 elements. ---
**Author:** ![FEAnalyst](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/feanalyst/32/688_2.png) [@FEAnalyst](https://prepomax.discourse.group/u/FEAnalyst)\ **Post date:** [September 15, 2026, 4:19pm UTC](https://prepomax.discourse.group/t/mesh-generation-error/3660/14 "2026-09-15T16:19:58Z")
With C3D8R and a tie constraint instead of a contact pair, it took 35 s to solve it: ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/7/75655fb499868e56e64852160e4531dd34686b1d.png)