# A new PrePoMax version v3.0.0 RC1 has been released **URL:** \ **Category:** News\ **Created:** [October 12, 2026, 8:35pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737 "2026-10-12T20:35:08Z")\ **Posts on this page:** 20\ **Page:** 1
**Author:** ![Matej](https://avatars.discourse-cdn.com/v4/letter/m/a698b9/32.png) [@Matej](https://prepomax.discourse.group/u/Matej)\ **Post date:** [October 12, 2026, 8:35pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/1 "2026-10-12T20:35:08Z")
A new release version of the PrePoMax contains the following FEM features (with regard to v2.6.0): **Scripting and automation** - Complete Python support: script execution, Python API help, recording a Python script in the command history and converting the command history to a Python script - MCP server support, so AI assistants can drive a PrePoMax session **Geometry** - Repairing CAD parts (sew, fix shape, remove small faces and edges, fuse faces, join edges) - Fusing solid bodies - Fusing CAD part faces that lie on one surface - Splitting solid geometry into cells and grouping solid cells - Splitting shell geometry - Offsetting the surfaces of a CAD part - OpenCascade 8.0.1 for visualization and the Netgen mesher **Meshing** - Automatic sweep meshing of single and multiple parts (including split source faces) - QuadWild mesher - Parallel meshing in Netgen (surfaces and subdomains) - Netgen shell meshing of STL parts; the Mmg mesher now has its own mesh setup item - Exporting mesh parts **Model** - Material based on engineering constants (lamina) - Joints based on rigid body/spring connections - Contact pair grouping by graph - Parameter descriptions and reordering of parameters in the parameter editor **Analysis and results** - Axisymmetric models report all results for 360° - Binary .frd files (Settings → Solver → CalculiX) - Improved result part mapping (part by part, input decks with additional elements) - History output from a user-defined table, merged outputs, an entry and XY data - Duplicating field and history outputs - Kinetic energy read from the .dat file and energy plots in the Progress tab for dynamic steps - Mass computation for parts and the assembly (Query) The list of all new features can be found at: [Version 3.0.0 – PrePoMax](https://prepomax.fs.um.si/version-3-0-0/) Download: [Downloads – PrePoMax](https://prepomax.fs.um.si/downloads/) ---
**Author:** ![Matej](https://avatars.discourse-cdn.com/v4/letter/m/a698b9/32.png) [@Matej](https://prepomax.discourse.group/u/Matej)\ **Post date:** [October 12, 2026, 8:37pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/2 "2026-10-12T20:37:34Z")
### Automatic mesh types In previous versions a solid part without a mesh setup item was always meshed with tetrahedra by Netgen. In v3.0.0 PrePoMax looks at the geometry of every part and meshes it with the most structured mesh it supports: - a solid with 5 or 6 three- or four-sided faces (a box or a prism) gets a **transfinite** hexahedral mesh, - a solid that can be swept from one set of faces to the opposite set gets a **swept** hexahedral mesh, - a solid that can be turned around an axis gets a **revolved** mesh, - all other solids are meshed with **tetrahedra** by Netgen, as before. CAD shell parts are meshed quad-dominant by Gmsh, with structured grids on three- and four-sided faces. You do not need any mesh setup item for this; just create the mesh. A mesh setup item you define yourself is always used instead of the automatic choice, so if you want tetrahedra, add a **Netgen Mesh** item to the part. Models saved with an older version are meshed as before. Their history gets a **Disable default mesh types** command, and the parts without a mesh setup item receive a Netgen Mesh item with their old settings. Delete that command from the history to switch the model to automatic mesh types. ### Seeing the mesh types before meshing Use **View → Color Annotations → Mesh Types** (or the _Color by_ box in the toolbar) to see what each part will be meshed with before you mesh it. Parts, and shell faces one by one, are colored as Transfinite, Sweep, Revolve, Tetrahedral or Free. The colors can be changed in **Settings → Colors**. While this annotation is on, the Output window explains, for every solid that will get tetrahedra, why it cannot be swept, naming the surface or the cell that blocks the sweep. This is the main tool for deciding where a part should be split (see below). ### Sweep meshing The Extrude and Revolve mesh setup items were replaced by a single **Sweep Mesh** item; old items are converted when a file is opened. With _Source surfaces = Automatic_ (the default) you only select the parts. PrePoMax finds the source faces and the sweep direction itself and shows them in the dialog with arrows. One item can sweep several parts; parts in a box selection that cannot be swept are skipped. The numbers of elements on connected edges are matched automatically, so the mesh stays conformal between neighboring cells. If the numbers of elements you set cannot all be satisfied, meshing stops, and **Preview Edge Mesh** highlights the conflicting edges and surfaces. The source faces can also be meshed with the new QuadWild quad mesher. ### Compound parts, sub parts and cells Until now, a compound part was created with **Create Compound Part** from several parts that touch each other. The parts are imprinted on each other, so the mesh is conformal where they meet, and each original part becomes a sub part. This still works as before. New in v3.0.0, a single part can be divided into **cells** with **Geometry → CAD Part → Split Solid**. The part can be cut by a plane (defined by three points or by a point and a normal), by an extended face, or by an extruded edge. The dialog has a preview and an undo button. After the split, the part keeps its name in the model tree, and its pieces are listed under it as cells (_Part-1\_cell-1_, _Part-1\_cell-2_, …). A **sub part** is the part as you think of it; a **cell** is one solid piece of it. Selecting, hiding, coloring or renaming a sub part acts on all of its cells. The cells share their faces and nodes, so the mesh is conformal. By default, all cells of a sub part are merged into one mesh part. Set _Merge cells_ to _No_ in the meshing parameters to get one mesh part per cell, for example to assign different sections. **Why are cells needed?** A complex solid can rarely be swept as one block, but its pieces often can. Split the part into sweepable cells, and PrePoMax sweeps each of them. Cells that still cannot be swept are filled with tetrahedra, with pyramids at the transition, and everything stays conformal. The usual workflow is: switch on the Mesh Types colors, look at the parts colored as tetrahedral, read the reason in the Output window, split, and repeat. The Split Solid dialog has a button that toggles the Mesh Types colors while you split. Two commands work on cells, and they are easy to confuse: - **Group Cells** does not change the geometry. It only collects the selected cells under one sub part, which becomes one mesh part (e.g. all cells that should be steel). - **Fuse Bodies** changes the geometry. The selected cells become one solid, and the faces between them are removed. Use it to undo an unwanted cut or to remove an interior face that spoils the mesh. Fusing all cells of a part gives back a plain part. Please note that splitting a plain part replaces it with a new compound part, so items that referred to the old part (selections, sections, loads, …) must be redefined. **Split the geometry before you build the model.** To divide only faces and not the body, for example to apply a load to a part of a face, use **Split Face**. **Fuse Faces** is its inverse. ### Parts with small features A CAD part now shows an icon with an orange exclamation mark in the model tree if it has an edge shorter than 1/1000 of the part’s bounding box diagonal, or a face narrower than that (a thin strip or sliver). Such features force very small elements around them, which slows meshing and spoils the element quality. They are often left behind by imported CAD, splitting or defeaturing. When you select the part, its small edges and their vertices are highlighted. Remove them with **Geometry → CAD Part → Repair** (remove small faces and edges, fuse faces, join edges), using _Preview_ to see what will be removed. Other options are **Fuse Faces** and **Defeature Solid**. ### Other meshing changes - **Mesh sizes are no longer changed silently.** A local element size or number of elements that conflicts with the minimum/maximum element size, or with a structured face, used to be quietly adjusted. Now meshing stops with a message that names the edges and surfaces. Older models may therefore report errors that they did not report before. - **Parallel Netgen meshing** has to be switched on in **Settings → Meshing → Number of threads** (the default is 1). The result is the same for any number of threads. A _Mesher time limit_ (30 min by default) stops meshers that hang. - The **Netgen Mesh** item (previously _Tetrahedral Netgen_) now contains the Netgen settings that used to be in the meshing parameters, plus transfinite options for three- and four-sided faces. - Open STL shells are now meshed by Netgen by default. The Mmg mesher has its own **Shell Mmg** mesh setup item for STL shell parts, and the Hausdorff settings moved there. - The _Grading_ parameter now also applies to Gmsh meshes, so fillets no longer fill a part with millions of elements. ### Periodic faces are no longer split on import A periodic face is a face that closes on itself along a single seam, such as the wall of a cylinder, a hole or a boss. Since v2.2.4, every CAD import split each periodic face into two or more faces, and every geometry operation (defeaturing, repair, compound parts, …) split it again. You reported import failures and parts that could no longer be defeatured, and the two halves of a cylinder could not be fused back into one face. The split was needed only by the sweep mesher, which now meshes such a wall around its seam. In v3.0.0, the wall of a hole stays **one face** after import. If you need it split, for example to apply a load to one half of a cylinder, use **Geometry → CAD Part → Split Periodic Faces** and enter the number of faces. The command keeps the part’s name, id and body. Once fused, faces stay fused, and defeaturing a hole no longer has to deal with its halves. Older files regenerate exactly as they were recorded, with the periodic faces split as before. This is controlled by **Settings → General → Regenerate older files → Split periodic faces** and _Number of resulting faces_. Note that in a new model, selections, loads or boundary conditions that relied on the halves of a cylinder must now be made on the whole face, or on faces created by Split Periodic Faces. ---
**Author:** ![Matej](https://avatars.discourse-cdn.com/v4/letter/m/a698b9/32.png) [@Matej](https://prepomax.discourse.group/u/Matej)\ **Post date:** [October 12, 2026, 8:42pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/3 "2026-10-12T20:42:07Z")
I expect most of the problems will be with parts that will not mesh using the sweepable mesh. To improve the mesher, I would need such parts for testing. So if you have a part that should sweep mesh (preferably confirmed by other tools) but does not, please share it with me. The .step file alone will suffice, since we are slowly running out of the 5 GB of free space on the forum. ---
**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:** [October 12, 2026, 9:16pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/4 "2026-10-12T21:16:32Z")
I don’t even know how to thank you for this incredible effort, but I guess I’ll just slowly start updating the manual to have it possibly on time with the stable release (whenever it happens, but I plan some vacation in November, so I’ll better start earlier this time). Maybe this stable release will happen close to FreeCAD 26.3 (they also published RC1 a few days ago). That would be the best early Christmas gift 😉 > [@Matej](#): > > I expect most of the problems will be with parts that will not mesh using the sweepable mesh. To improve the mesher, I would need such parts for testing. Such a huge amount of features/changes will indeed require quite extensive testing. Especially the automated/unified meshing and maybe also partition-related stuff. I will try to test as much as possible. > [@Matej](#): > > The .step file alone will suffice, since we are slowly running out of the 5 GB of free space on the forum. Perhaps it would make sense to delete some older and larger files, especially since they won’t open in new versions of PrePoMax. But also, we could use our new Discord server and maybe a desicated GitHub repo. They shouldn’t have any restrictions on the total storage capacity. Of course, we could also use hosting services more, even the temporary ones since those files won’t be needed in the future. ---
**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:** [October 13, 2026, 3:51am UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/5 "2026-10-13T03:51:32Z")
Amazing update, the new part spliting tools and hexa meshing are awesome! ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/8/8ba54dc2a861e3b9901e60b6ff91cbdb42dd3eb2.jpeg) ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/f/f1c3808c69f0e6f6539ada7bb56f580f44ac7717.jpeg) ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/f/f71a5d4e8206a9aa6aeb751586407310b1919949.jpeg) ---
**Author:** ![Matej](https://avatars.discourse-cdn.com/v4/letter/m/a698b9/32.png) [@Matej](https://prepomax.discourse.group/u/Matej)\ **Post date:** [October 13, 2026, 6:33am UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/6 "2026-10-13T06:33:50Z")
> [@FEAnalyst](#): > > I don’t even know how to thank you for this incredible effort, but I guess I’ll just slowly start updating the manual to have it possibly on time with the stable release (whenever it happens, but I plan some vacation in November, so I’ll better start earlier this time). Dear @FEAnalyst, I should be the one thanking you for all the work on the forum, documentation, and now Discord. There is no need for haste in documentation preparation. Take your time. ---
**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:** [October 13, 2026, 7:40am UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/7 "2026-10-13T07:40:53Z")
Simple example first: 1. Original model: ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/9/9e8b55aad8c5edfc5f21d31ad9c2fa471d7fb120.png) 1. Defeatured model (thanks for the selection improvements in the defeaturing tool): ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/6/6090092f215f273bacfe451f7495a22deefb11f6.png) 1. Partitioned model: ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/9/9806be283f9450da81d905879b2057607a797600.png) 1. Meshed model: ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/5/5c12d7fc803c0558941b49c8c4599eada47c89a1.jpeg) ---
**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:** [October 13, 2026, 1:32pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/8 "2026-10-13T13:32:39Z")
Hi @Matej , this is my first try to mesh a rubber bush, but including all the radius and draft angles as it should be to get accurate stress. I have modeled the part in FreeCAD and there I made the partitions, happily Prepomax has found a way to mesh most of them, but some of them should be treated separately: ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/7/73c076b49e9cd2db6fe1b4b2c442eb1f949c2290.png) In this volume, I guess that others meshers would made the sweep, I don´t have available Abaqus or Siemens NX to test by my self: ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/e/ef393d52b3884b5b008fbf1376e6f9634963249a.png) This is the second volume, if the first one were sweeped in vertical direction, then this should be done tangential direction to use the same face mesh from the last one, but cannot be done ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/1/1c5319a57f87a873084cdbecfd09e81a99d6424d.png) this volume can be meshed sweeping from the upper faces, but that would lock the mesh of the first volume: ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/e/e13519c0db72fc2e6d84b00bb2ff6efcd15a62ac.png) I´m attaching the model and native CAD file so everyone can play with it, is a nice mesh exercise. Back to the first volume, I made some more partitions in PPM ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/7/73ec6a5e14797d955d0f50d05872cbef26a830db.png) and I think that the middle volume could be swepped vertically from the curved face to the planar one… no success in PPM, but works from the lower side! ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/0/02bc74ff858fa03335ede6da9c2377bb9cbf12ad.png) ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/7/7a1fccda0948ff25d515dfb564d04f158e5279d4.png) But how could I join all the volumes to force the conformal meshing? ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/a/a0fa8358dc4881d46168e04bca67a24368d74879.png) [RUBBER BUSH.pmx](https://prepomax.discourse.group/uploads/short-url/tNrURIT2kRWqw95bfgjHUQ39IWh.pmx) (1.9 MB) [RUBBER BUSH.zip](https://prepomax.discourse.group/uploads/short-url/i39vidtTnhET4G9DJAoYhE3gcoL.zip) (3.0 MB) ---
**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:** [October 13, 2026, 1:48pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/9 "2026-10-13T13:48:49Z")
> [@SergioP1975](#): > > In this volume, I guess that others meshers would made the sweep, I don´t have available Abaqus or Siemens NX to test by my self: Abaqus also can’t mesh this segment without further modifications: ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/c/cd8cc330cd944155f3270021be09788356c073bf.png) > [@SergioP1975](#): > > This is the second volume, if the first one were sweeped in vertical direction, then this should be done tangential direction to use the same face mesh from the last one, but cannot be done Abaqus can sweep this one tangentially: ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/7/77acc05cff6af460e6fc09e6ae7721ef9b95298b.png) ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/f/f161690e91f2149cc1000bbfc7acbd08a1850195.png) ---
**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:** [October 13, 2026, 2:16pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/10 "2026-10-13T14:16:28Z")
Hi, thanks for the support. How could I join all the volumes to get a conformal mesh? ---
**Author:** ![Fran](https://avatars.discourse-cdn.com/v4/letter/f/a4c791/32.png) [@Fran](https://prepomax.discourse.group/u/Fran)\ **Post date:** [October 13, 2026, 2:33pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/11 "2026-10-13T14:33:38Z")
Wow this update looks awesome! I was able to open it this morning, but now not anymore. I get the following error, which says that the path cannot be accessed and that I don’t have the required permissions, although the other versions of PPM have the same path and open perfectly. ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/3/34087d8c1096ff666daa7cd0222a495d1050886a.png) My company recently switched to Windows 11 365, maybe it is related. I tried running PPM from a non-OneDrive folder but I get the same error. I tried rebooting but it has no effect. Also, when I was able to open it this morning, I quickly opened an pmx file made with 2.6.0 and tried to mesh a part. It failed and it was written in the console “Part 50: Zugriff verweigert” (yes with text in German in the middle of the usual text in English, my Windows system is in German) which means “Access denied”. I then tried to mesh this part again as well as other parts, but then got the message “Part XX is already being meshed” (or something similar). ---
**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:** [October 13, 2026, 2:46pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/12 "2026-10-13T14:46:40Z")
I got a mesh!!! Ugly as hell, but is a begining, has to work with the partitions and local refinements to get a better distribution and less deformation of the elements. Thanks @Matej for this wonderfull update ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/c/cb192dc5670dde53a73c6955e8ffd7387bbb61f2.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:** [October 13, 2026, 3:15pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/13 "2026-10-13T15:15:03Z")
Yeah, you may need many cuts for such geometries with fillets, also in Abaqus. @Fran PrePoMax should always be placed in a Windows directory that doesn’t require admin rights. You may need to avoid paths with non-ASCII characters too. Same with the work directory where PrePoMax writes all files. ---
**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:** [October 13, 2026, 3:17pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/14 "2026-10-13T15:17:34Z")
But can be meshed the part in steps as we would do in NX? there I would start meshing the middle volumen, and then advancing to the others, but one by one to see how the mesh behave. ---
**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:** [October 13, 2026, 3:23pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/15 "2026-10-13T15:23:05Z")
Yes, the algorithm is assigned automatically (you can switch between structured, sweep and tetra if applicable and change the sweep direction, though). But you can mesh cells one-by-one - there is an option to mesh only selected regions. Still, it has to be within one part object to obtain a continuous mesh. ---
**Author:** ![Fran](https://avatars.discourse-cdn.com/v4/letter/f/a4c791/32.png) [@Fran](https://prepomax.discourse.group/u/Fran)\ **Post date:** [October 13, 2026, 3:26pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/16 "2026-10-13T15:26:16Z")
Thanks for your suggestions. I checked that and the directories I use don’t require admin rights and the paths don’t contain non-ASCII characters.. ---
**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:** [October 13, 2026, 3:35pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/17 "2026-10-13T15:35:37Z")
Can you try a different folder just in case ? I see that you use the Documents folder, so maybe try a different drive (if you have it) or Program Files on C. ---
**Author:** ![Fran](https://avatars.discourse-cdn.com/v4/letter/f/a4c791/32.png) [@Fran](https://prepomax.discourse.group/u/Fran)\ **Post date:** [October 13, 2026, 3:56pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/18 "2026-10-13T15:56:01Z")
I tried running from the following folders: - C:\PrePoMax\PrePoMax v3.0.0 RC1 - C:\user\…\Documents\PrePoMax\PrePoMax v3.0.0 RC1 - D:\PrePoMax\PrePoMax v3.0.0 RC1 (other local drive) - A network drive - the OneDrive folder - the Desktop (which is actually also part of the OneDrive folder) - A USB-stick I got the same error in all cases. I couldn’t place PPM in Program Files because this require admin rights. ---
**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:** [October 13, 2026, 4:22pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/19 "2026-10-13T16:22:36Z")
I have created a compound with my original partitions made in FreeCAD and the new ones made in PPM, so I can mesh it all in one operation: ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/1/15a036105dd062383a1f5fc303012b699d06e277.png) But if I want to mesh by volumes starting from one of them, there is no option to mesh separately. I´m missing something? ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/b/b61505892a41484eb36753d57106410e5b38f882.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:** [October 13, 2026, 4:27pm UTC](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737/20 "2026-10-13T16:27:01Z")
Selective cell meshing in Abaqus/CAE: ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/0/0b64a460367c46580babeb77efa516f49c18f833.png) ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/f/f76de55f77c17d126e3f0a6423ceadd06bad0db3.png) In PrePoMax, the only way seems to be this: > [@Matej](#): > > By default, all cells of a sub part are merged into one mesh part. Set _Merge cells_ to _No_ in the meshing parameters to get one mesh part per cell, for example to assign different sections. [Next page](https://prepomax.discourse.group/t/a-new-prepomax-version-v3-0-0-rc1-has-been-released/3737.md?page=2)