# Insertion and withdrawal force calculation with plastic deformation **URL:** \ **Category:** General Questions\ **Created:** [November 17, 2025, 2:28pm UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097 "2025-11-17T14:28:08Z")\ **Posts on this page:** 20\ **Page:** 2
**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:** [November 20, 2025, 2:16pm UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/21 "2025-11-20T14:16:49Z")
> [@synt](#): > > my experiences shown PaStiX is faster than Pardiso in case of large contact and plasticity. Good to know, I stick to Pardiso because it’s the default solver in PrePoMax and has less issues (e.g. with eigenvalue analyses). > [@synt](#): > > any example models were Mortar contact fails? it’s promoted by many to be robust and accurate in contact analysis, unfortunately Abaqus and Ansys seems not have. Nothing specific, I just tried it a few times in different cases and it didn’t work well. It seems to be an equivalent of lagrange multipliers contact in Abaqus which is not recommended in most cases due to convergence difficulties and longer calculations. It’s more accurate than penalty contact though. ---
**Author:** ![BliTec](https://avatars.discourse-cdn.com/v4/letter/b/ecccb3/32.png) [@BliTec](https://prepomax.discourse.group/u/BliTec)\ **Post date:** [November 20, 2025, 2:55pm UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/22 "2025-11-20T14:55:13Z")
I have played with different values for contact stiffness. See previous pictures. This setup gives the best solution; the graph of insertion shows the most realistic graph of the insertion force. The amount of allowed penetration is not clear. ---
**Author:** ![BliTec](https://avatars.discourse-cdn.com/v4/letter/b/ecccb3/32.png) [@BliTec](https://prepomax.discourse.group/u/BliTec)\ **Post date:** [November 20, 2025, 2:59pm UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/23 "2025-11-20T14:59:29Z")
Running with “HARD” setting for surface behavior shows this : \*WARNING reading \*SURFACE BEHAVIOR: K must be strictly positive the following default will be used: 1125000.0000000000 the user is advised to analyze the results carefully ---
**Author:** ![BliTec](https://avatars.discourse-cdn.com/v4/letter/b/ecccb3/32.png) [@BliTec](https://prepomax.discourse.group/u/BliTec)\ **Post date:** [November 20, 2025, 3:12pm UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/24 "2025-11-20T15:12:33Z")
I have reduced the mesh size of EON. Runned with 2 steps with Pardiso Solver with hard surface behavior. This looks ok. ![afbeelding](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/a/ade7740f96560746f3e93e4c7ce263c18356698d.png) Still lot of penetration ![afbeelding](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/3/300c50eb55d0ca94a0ae08b974aa0f1976be84b2.png) Now to do simulation with friction. ---
**Author:** ![BliTec](https://avatars.discourse-cdn.com/v4/letter/b/ecccb3/32.png) [@BliTec](https://prepomax.discourse.group/u/BliTec)\ **Post date:** [November 20, 2025, 3:14pm UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/25 "2025-11-20T15:14:51Z")
What penetration depth do you have in this simulation? ---
**Author:** ![BliTec](https://avatars.discourse-cdn.com/v4/letter/b/ecccb3/32.png) [@BliTec](https://prepomax.discourse.group/u/BliTec)\ **Post date:** [November 20, 2025, 3:55pm UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/26 "2025-11-20T15:55:00Z")
Same simulation, but now with friction. ![afbeelding](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/0/07149d8c3a79ede8a26c93a0f9bc75f8aca920d5.png) Error at time step 0.6s \*ERROR: too many cutbacks best solution and residuals are in the frd file Process elapsed time: 1104.364 s ![afbeelding](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/7/788acd124a4f5306d3d7286d2ac379b45b883068.png) ---
**Author:** ![synt](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/synt/32/4658_2.png) [@synt](https://prepomax.discourse.group/u/synt)\ **Post date:** [November 20, 2025, 4:44pm UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/27 "2025-11-20T16:44:35Z")
the value is 0.7mm(negative) or 0.8mm maybe, i lost my model files. ---
**Author:** ![BliTec](https://avatars.discourse-cdn.com/v4/letter/b/ecccb3/32.png) [@BliTec](https://prepomax.discourse.group/u/BliTec)\ **Post date:** [November 21, 2025, 8:28am UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/28 "2025-11-21T08:28:56Z")
Here are the files. With and without friction. Can you tell me what to do to get it done with friction? [contact\_005-54-io-p\_2\_steps\_share-7.pmx](https://prepomax.discourse.group/uploads/short-url/78Ax31Y4Dfd7yTy10Mjcf18y44C.pmx) (5.9 MB) [contact\_005-54-io-p\_2\_steps\_share-7-F.pmx](https://prepomax.discourse.group/uploads/short-url/iZIdEJp35xBLguSzR3s3dLcDt6R.pmx) (6.0 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:** [November 21, 2025, 10:06am UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/29 "2025-11-21T10:06:11Z")
> [@BliTec](#): > > Here are the files. With and without friction. > > Can you tell me what to do to get it done with friction? Whether it’s frictional or frictionless contact, you still have large penetration. This has to be resolved by adding a small fillet to the edge od the PCB part, further refining the mesh locally (possibly, in a smaller region) or changing the contact settings. ---
**Author:** ![BliTec](https://avatars.discourse-cdn.com/v4/letter/b/ecccb3/32.png) [@BliTec](https://prepomax.discourse.group/u/BliTec)\ **Post date:** [November 21, 2025, 10:14am UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/30 "2025-11-21T10:14:34Z")
Is there a optimum ratio between cells of the slave and master mesh to have less penetration? ---
**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:** [November 21, 2025, 12:33pm UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/31 "2025-11-21T12:33:36Z")
Not really, but here the problem is more specific. You have a sharp corner, and it’s hard for the solver to properly establish contact between that edge and the rounded surface of the clip. In Abaqus, you could use a separate node-to-surface pair for that. Here, it might be best to just add a fillet to that sharp corner (and refine it properly). Adding more fillets is what helped resolve the issue with snap fit analysis described in the referenced CalculiX forum thread. ---
**Author:** ![BliTec](https://avatars.discourse-cdn.com/v4/letter/b/ecccb3/32.png) [@BliTec](https://prepomax.discourse.group/u/BliTec)\ **Post date:** [November 21, 2025, 12:55pm UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/32 "2025-11-21T12:55:59Z")
Thanks. I will do that ---
**Author:** ![BliTec](https://avatars.discourse-cdn.com/v4/letter/b/ecccb3/32.png) [@BliTec](https://prepomax.discourse.group/u/BliTec)\ **Post date:** [November 24, 2025, 1:03pm UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/34 "2025-11-24T13:03:40Z")
I have made a new model. Reduced the mesh size of the EON and added a radius on the edge of the copper-plated hole in the PCB. Only the material of the EON has plastic properties. The copper only has linear properties to see if the simulation will run. ![afbeelding](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/0/058d9c457d554cb13b60e0c812c72786fa58d4e8.jpeg) The simulation runs up to 1.3s of the 2s ![afbeelding](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/6/65c879d4550a03ddc2ce8dbe3d821aca715b6ebd.png) ![afbeelding](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/0/0e5e790d2141e4af36f872096050e7f7d78ed021.jpeg) Like to run with copper with plastic properties too, but that results in an ERROR. [EON\_10103550\_FEA\_001\_06-P.pmx](https://prepomax.discourse.group/uploads/short-url/22IFsv5tjXDoyJLH4manf35Vdab.pmx) (6.6 MB) Question: How do I TIE the copper to the PCB inthe right way? ---
**Author:** ![Vitek\_SAA](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/vitek_saa/32/6106_2.png) [@Vitek\_SAA](https://prepomax.discourse.group/u/Vitek_SAA)\ **Post date:** [November 27, 2025, 8:17am UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/35 "2025-11-27T08:17:46Z")
> [@BliTec](#): > > Question: How do I TIE the copper to the PCB inthe right way? I am not entirely sure about the exact properties of the Copper-PCB interface. However, regarding the tie definition, I would suggest using a compound part with distinct material assignments. Please see the attached images for reference. ![Snímek obrazovky 2025-11-27 091433](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/8/842687deda195e847a57d37feb62542b2e37e894.png) ![Snímek obrazovky 2025-11-27 091444](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/5/526976c6ee5738eb6d49ec14e5e5fbc7b9789daa.png) ---
**Author:** ![ANYS](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/anys/32/7737_2.png) [@ANYS](https://prepomax.discourse.group/u/ANYS)\ **Post date:** [November 27, 2025, 9:02am UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/36 "2025-11-27T09:02:25Z")
Regarding initial penetration and inspection of the load path be aware that ccx could be relaxing the contact stiffness to help for convergence and only at the end of the timestep it is increased to it’s requested value. For problems like this it could completely change the reaction and contact pressure response during the insertion and later withdrawal. ---
**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:** [November 27, 2025, 9:11am UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/37 "2025-11-27T09:11:03Z")
A workaround could be to a dummy step: [Snap-fit contact snagging problem - #20 by SergioP - CalculiX (official versions are on www.calculix.de, the official GitHub repository is at https://github.com/Dhondtguido/CalculiX).](https://calculix.discourse.group/t/snap-fit-contact-snagging-problem/2277/20) ---
**Author:** ![BliTec](https://avatars.discourse-cdn.com/v4/letter/b/ecccb3/32.png) [@BliTec](https://prepomax.discourse.group/u/BliTec)\ **Post date:** [November 27, 2025, 11:30am UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/38 "2025-11-27T11:30:18Z")
Thanks. I will try this. ---
**Author:** ![BliTec](https://avatars.discourse-cdn.com/v4/letter/b/ecccb3/32.png) [@BliTec](https://prepomax.discourse.group/u/BliTec)\ **Post date:** [November 27, 2025, 11:40am UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/39 "2025-11-27T11:40:20Z")
If you choose HARD, then it relaxes, but I haven’t seen it when linear with defined stiffness was selected in the monitor output. But further down the insertion, you see the deformation, and it seems then their the relaxation takes place. ---
**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:** [November 27, 2025, 11:54am UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/40 "2025-11-27T11:54:20Z")
Maybe you could also try the exponential definition: ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/7/7d14db1392d31c0647ab0dab97dcf0a1d126adb9.png) ---
**Author:** ![BliTec](https://avatars.discourse-cdn.com/v4/letter/b/ecccb3/32.png) [@BliTec](https://prepomax.discourse.group/u/BliTec)\ **Post date:** [November 27, 2025, 1:09pm UTC](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097/41 "2025-11-27T13:09:31Z")
I have re-modeld the pcb with the copper bushing with smaller mesh. Also made the displacemant of the contact insertion very small. I think that you have to make the step displacement smaller or equal to the mesh size of the slave to get it running. The copper bushing and the contact are both materials with plastic properties. ![afbeelding](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/d/d82d0bd4455b57bef5298e7a76665fe5918b775f.png) It runs now well until a depth of 0.165mm then it . _divergence allowed: residual force too large_ _divergence; the increment size is decreased to 9.765625e-06_ _the increment is reattempted_ ![afbeelding](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/e/ec570b1583c53881a1f0ee9918f6e9b08eeaa2c8.png) ![afbeelding](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/1/117bae98aa6cf9214184d68af536f1c7e1efffe9.jpeg) to be continued [Previous page](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097.md?page=1) [Next page](https://prepomax.discourse.group/t/insertion-and-withdrawal-force-calculation-with-plastic-deformation/3097.md?page=3)