# Contact analysis won't run **URL:** \ **Category:** General Questions\ **Created:** [October 10, 2023, 8:14am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163 "2023-10-10T08:14:42Z")\ **Posts on this page:** 20\ **Page:** 1
**Author:** ![tMKP](https://avatars.discourse-cdn.com/v4/letter/t/0ea827/32.png) [@tMKP](https://prepomax.discourse.group/u/tMKP)\ **Post date:** [October 10, 2023, 8:14am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/1 "2023-10-10T08:14:42Z")
![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/f/f8fce4c4c017b848b6045e5e01c4e99a5676239c.png) > **[FEA Pelat Penggantung - 0.6 better mesh.pmx](https://drive.google.com/file/d/197ylvlgw2ZN-1JNhaAaJGRKa2Ff9THRe/view?usp=sharing)** > > Google Drive file. I created this model to test pin-hanger contact analysis in PrePoMax. Sadly, the model would not run, and I don’t know what the problem is. Thank you in advance. ---
**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 10, 2023, 9:03am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/2 "2023-10-10T09:03:55Z")
What do you mean by “won’t run” ? Is there an error after some time after submitting the analysis or it just runs for a very long time ? When I remove the mesh refinements to run quick tests, the analysis is solved so maybe you just refined the mesh too much for your computer’s capabilities. ---
**Author:** ![tMKP](https://avatars.discourse-cdn.com/v4/letter/t/0ea827/32.png) [@tMKP](https://prepomax.discourse.group/u/tMKP)\ **Post date:** [October 10, 2023, 9:21am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/3 "2023-10-10T09:21:51Z")
Thanks for your reply. I already tried test runs without mesh refinements yesterday as you said before. The results were not as I expected. Bearing stresses incomparably larger (2 to 3 times) and differs too greatly with ANSYS. The same model (with 2 mm mesh refinement) would solved in 2 to 3 minutes runtime in ANSYS. My PC is using i7-13700KF and 64GB of DDR5 RAM. Even when only using mesh refinement dimension of 4 mm, this model will not run. By I mean “won’t run” is it stuck at iteration 1 not utilizing that much of my CPU. ---
**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 10, 2023, 9:28am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/4 "2023-10-10T09:28:17Z")
Are you using parallel processing ? This processor has 16 cores and you should set this in PrePoMax. ---
**Author:** ![tMKP](https://avatars.discourse-cdn.com/v4/letter/t/0ea827/32.png) [@tMKP](https://prepomax.discourse.group/u/tMKP)\ **Post date:** [October 10, 2023, 9:30am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/5 "2023-10-10T09:30:36Z")
Yes, I’m aware of it. I also use these keywords since earlier this year: |OPENBLAS\_NUM\_THREADS|1| |PASTIX\_MIXED\_PRECISION|1| ---
**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 10, 2023, 9:32am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/6 "2023-10-10T09:32:15Z")
And it shows 16 cpus in the job monitor ? You could also try using Pardiso instead of the default PaStiX, it can be even faster and more reliable. ---
**Author:** ![tMKP](https://avatars.discourse-cdn.com/v4/letter/t/0ea827/32.png) [@tMKP](https://prepomax.discourse.group/u/tMKP)\ **Post date:** [October 10, 2023, 9:42am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/7 "2023-10-10T09:42:55Z")
> 10/10/2023 16:39:33 > > ######## Starting run step number: 1 Increment number: 1 ######## > > Running command: C:\Program Files\PrePoMax v1.4.1\Solver\ccx\_static.exe Analysis-1 > > * * * > > CalculiX Version 2.21, Copyright(C) 1998-2023 Guido Dhondt > CalculiX comes with ABSOLUTELY NO WARRANTY. This is free > software, and you are welcome to redistribute it under > certain conditions, see gpl.htm > > * * * > > You are using an executable made on Sat Jul 29 17:18:34 2023 > > The numbers below are estimated upper bounds > > number of: > > nodes: 588702 > elements: 348993 > one-dimensional elements: 0 > two-dimensional elements: 0 > integration points per element: 4 > degrees of freedom per node: 3 > layers per element: 1 > > distributed facial loads: 8 > distributed volumetric loads: 0 > concentrated loads: 0 > single point constraints: 26742 > multiple point constraints: 1 > terms in all multiple point constraints: 1 > tie constraints: 1 > dependent nodes tied by cyclic constraints: 0 > dependent nodes in pre-tension constraints: 0 > > sets: 22 > terms in all sets: 1379721 > > materials: 2 > constants per material and temperature: 8 > temperature points per material: 1 > plastic data points per material: 0 > > orientations: 0 > amplitudes: 6 > data points in all amplitudes: 6 > print requests: 0 > transformations: 0 > property cards: 0 > > \*WARNING reading \*FRICTION: stick slope > must be strictly positive > the following default will be used: 105000.00000000000 > the user is advised to analyze the results > carefully and, if possible, to come up with > a experimentally based stick slope > \*WARNING reading \*FRICTION. Card image: > 0.2 > > STEP 1 > > \*INFO reading \*STEP: nonlinear geometric > effects are turned on > > Static analysis was selected > > Newton-Raphson iterative procedure is active > > Nonlinear geometric effects are taken into account There’s no such thing in job monitor. I read somewhere that I should compile the Pardiso solver manually? ---
**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 10, 2023, 9:48am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/8 "2023-10-10T09:48:03Z")
> [@tMKP](#): > > There’s no such thing in job monitor. Apparently, it didn’t get to that stage yet. Maybe try reducing the mesh refinement until it runs in a reasonable time (at least completes the first iteration). > [@tMKP](#): > > I read somewhere that I should compile the Pardiso solver manually? No need to. You can download it (with all the necessary libraries) from here: [https://staff.tu.kielce.pl/rokach/instr/misc/ccx\_220.7z](https://staff.tu.kielce.pl/rokach/instr/misc/ccx_220.7z) ---
**Author:** ![tMKP](https://avatars.discourse-cdn.com/v4/letter/t/0ea827/32.png) [@tMKP](https://prepomax.discourse.group/u/tMKP)\ **Post date:** [October 10, 2023, 10:21am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/9 "2023-10-10T10:21:34Z")
> Maybe try reducing the mesh refinement until it runs in a reasonable time (at least completes the first iteration). The smallest I could get is 5 mm. ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/a/ad72b18cb237985f5e404e23733c2973da18b0d8.png) And there is still these unexpected stress concentration as shown in output above. I expected the stress distribution to be somewhat linear (like strips) with maximum of 1100 MPa. Using Pardiso greatly improves calculation time. ```auto 10/10/2023 17:13:37 ######## Starting run step number: 1 Increment number: 1 ######## Running command: C:\Program Files\PrePoMax v1.4.1\Solver\ccx_dynamic.exe Analysis-1 ************************************************************ CalculiX Version 2.20, Copyright(C) 1998-2022 Guido Dhondt CalculiX comes with ABSOLUTELY NO WARRANTY. This is free software, and you are welcome to redistribute it under certain conditions, see gpl.htm ************************************************************ You are using an executable made on Sun Jul 31 22:11:42 2022 The numbers below are estimated upper bounds number of: nodes: 181662 elements: 102665 one-dimensional elements: 0 two-dimensional elements: 0 integration points per element: 4 degrees of freedom per node: 3 layers per element: 1 distributed facial loads: 8 distributed volumetric loads: 0 concentrated loads: 0 single point constraints: 12432 multiple point constraints: 1 terms in all multiple point constraints: 1 tie constraints: 1 dependent nodes tied by cyclic constraints: 0 dependent nodes in pre-tension constraints: 0 sets: 23 terms in all sets: 368663 materials: 2 constants per material and temperature: 8 temperature points per material: 1 plastic data points per material: 0 orientations: 0 amplitudes: 6 data points in all amplitudes: 6 print requests: 0 transformations: 0 property cards: 0 *WARNING reading *FRICTION: stick slope must be strictly positive the following default will be used: 105000.00000000000 the user is advised to analyze the results carefully and, if possible, to come up with a experimentally based stick slope *WARNING reading *FRICTION. Card image: 0.2 *INFO reading *STEP: nonlinear geometric effects are turned on STEP 1 Static analysis was selected Newton-Raphson iterative procedure is active Nonlinear geometric effects are taken into account Decascading the MPC's Determining the structure of the matrix: Using up to 16 cpu(s) for setting up the structure of the matrix. number of equations 433692 number of nonzero lower triangular matrix elements 15707109 increment 1 attempt 1 increment size= 1.000000e+00 sum of previous increments=0.000000e+00 actual step time=1.000000e+00 actual total time=1.000000e+00 iteration 1 Number of contact spring elements=919778 Determining the structure of the matrix: maximal possible contact elements = 1872437 Using up to 16 cpu(s) for setting up the structure of the matrix. number of equations 433692 number of nonzero lower triangular matrix elements 19554087 Using up to 16 cpu(s) for the stress calculation. Using up to 16 cpu(s) for the symmetric stiffness/mass contributions. Using up to 16 cpu(s) for the asymmetric stiffness/mass contributions. Factoring the system of equations using the unsymmetric pardiso solver number of threads = 16 Using up to 16 cpu(s) for the stress calculation. average force= 79.362623 time avg. forc= 79.362623 largest residual force= 20599.745536 in node 43154 and dof 2 largest increment of disp= 3.337239e+00 largest correction to disp= 3.337239e+00 in node 35202 and dof 2 no convergence iteration 2 Number of contact spring elements=528302 Using up to 16 cpu(s) for the stress calculation. Using up to 16 cpu(s) for the symmetric stiffness/mass contributions. Using up to 16 cpu(s) for the asymmetric stiffness/mass contributions. Factoring the system of equations using the unsymmetric pardiso solver number of threads = 16 Using up to 16 cpu(s) for the stress calculation. line search factor=0.951817 Using up to 16 cpu(s) for the stress calculation. average force= 138.070703 time avg. forc= 138.070703 largest residual force= 333717.981676 in node 118556 and dof 2 largest increment of disp= 3.337239e+00 largest correction to disp= 3.879927e-02 in node 41196 and dof 3 no convergence iteration 3 Number of contact spring elements=286235 Using up to 16 cpu(s) for the stress calculation. Using up to 16 cpu(s) for the symmetric stiffness/mass contributions. Using up to 16 cpu(s) for the asymmetric stiffness/mass contributions. Factoring the system of equations using the unsymmetric pardiso solver number of threads = 16 Using up to 16 cpu(s) for the stress calculation. line search factor=0.662338 Using up to 16 cpu(s) for the stress calculation. average force= 181.062673 time avg. forc= 181.062673 largest residual force= 120237.189560 in node 51733 and dof 1 largest increment of disp= 3.337239e+00 largest correction to disp= 4.118562e-02 in node 41126 and dof 3 ``` I found out if I try to use super small mesh refinement. The Analysis would _stuck_ like before for a long time, and then finally going into iteration steps after minutes. ---
**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 10, 2023, 10:30am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/10 "2023-10-10T10:30:47Z")
> [@tMKP](#): > > I found out if I try to use super small mesh refinement. The Analysis would _stuck_ like before for a long time, and then finally going into iteration steps after minutes. Yeah, CalculiX may still have issues with very large meshes. They were reported on the CalculiX forum multiple times. Fortunately, Pardiso is usually sufficient. ---
**Author:** ![tMKP](https://avatars.discourse-cdn.com/v4/letter/t/0ea827/32.png) [@tMKP](https://prepomax.discourse.group/u/tMKP)\ **Post date:** [October 10, 2023, 10:35am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/11 "2023-10-10T10:35:19Z")
Is there any explanation on why there exist such stress inaccuracies from Calculix on those bearing locations? And also in this case (cylindrical pin connection) is Calculix not suitable to simulate this problem? ---
**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:** [October 10, 2023, 11:21am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/12 "2023-10-10T11:21:39Z")
> [@tMKP](#): > > Is there any explanation on why there exist such stress inaccuracies from Calculix on those bearing locations? all CalculiX contact algorithm has been tested and benchmarked with well known solver Abaqus, it has shown good agreement. > [@tMKP](#): > > And also in this case (cylindrical pin connection) is Calculix not suitable to simulate this problem? i frequently used large set of bolt with contact analysis, even with medium mesh density still get reliable results compared to experimental test. try to swith to nonlinear material, the Mises stress you shown have ten times and more of it’s yield strength, thus make it unrealistic simulations. ---
**Author:** ![Matej](https://avatars.discourse-cdn.com/v4/letter/m/a698b9/32.png) [@Matej](https://prepomax.discourse.group/u/Matej)\ **Post date:** [October 10, 2023, 11:51am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/13 "2023-10-10T11:51:51Z")
You can also try to reduce the contact stiffness. This will increase the contact area and reduce the singularity effect of single-point contact. ---
**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:** [October 10, 2023, 1:02pm UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/14 "2023-10-10T13:02:16Z")
Faces have some interference. I would try to adjust midside nodes to the geometry and locate all the nodes on a common circle or maybe add some small clearance to speed up the process. ![screenshot.9](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/6/69e59bddce6aad9593536d1a8e834bb06839a790.jpeg) With overlaping surfaces and depending on the contact settings you could be solving an interference fit before loading. That is a lot of time if it is not intended. Note: I think boundary conditions on the bolt surfaces could be switched. (Symmetry / Fixed) ---
**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:** [October 10, 2023, 2:42pm UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/15 "2023-10-10T14:42:38Z")
indeed, i guessed there’s something missing or improperly defined in models, but i’m not yet to check since the file sizes are too large (35Mb), strange cases for model of single pins are unsolved by 64Gb of memory. ![2023-10-10 21_34_33-FEA Pelat Penggantung - 0.6 better mesh.pmx - Google Drive](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/8/86ebfaa3c56a332b45c51d9533a672a15a387303.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 10, 2023, 5:23pm UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/16 "2023-10-10T17:23:18Z")
> [@ANYS](#): > > With overlaping surfaces and depending on the contact settings you could be solving an interference fit before loading. That is a lot of time if it is not intended. Strain-free adjustment should be able to resolve such small initial overclosures before the actual analysis. ---
**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:** [October 11, 2023, 8:18am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/17 "2023-10-11T08:18:00Z")
I have adjust midside nodes to the geometry and provide an small minimum clearance . It helps to reduce peak stresses and computation time. I have consider displacement driven instead of force driven (like in a tensile test). Done on my 16 Gb RAM Laptop. ![screenshot.3](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/a/a3030d63818c149fe829642cded5f25258015ce6.jpeg) ![screenshot.5](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/0/0ee3e8416fb248a745c3717d30b5f9899fe38a80.jpeg) ![screenshot.4](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/2/28f69c17fd3a366a61bf40da77fec206baba37ca.jpeg) ---
**Author:** ![tMKP](https://avatars.discourse-cdn.com/v4/letter/t/0ea827/32.png) [@tMKP](https://prepomax.discourse.group/u/tMKP)\ **Post date:** [October 12, 2023, 6:47am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/18 "2023-10-12T06:47:28Z")
> Note: I think boundary conditions on the bolt surfaces could be switched. (Symmetry / Fixed) I thought applying 0 mm DOF is the same as symmetry? As I watched the chain link tutorial on FEAnalyst YouTube video. > I have adjust midside nodes to the geometry Do you mean “Midside nodes on geometry”? and > provide an small minimum clearance Where can I apply this? ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/7/7f318ec0e9dd0655de637701ee91706798022594.png) This is the previous result I got from ANSYS. Maximum von-Mises Stress is 1021 MPa ---
**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, 2023, 7:46am UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/19 "2023-10-12T07:46:43Z")
> [@tMKP](#): > > I thought applying 0 mm DOF is the same as symmetry? There’s no predefined symmetry BC in PrePoMax but setting displacements in the normal direction to zero is the same (at least for solids). However, I think that ANYS meant just switching places so defining symmetry where fully fixed BC was and vice versa. > [@tMKP](#): > > Where can I apply this? You would have to modify the geometry before importing it to PrePoMax. ---
**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:** [October 12, 2023, 9:34pm UTC](https://prepomax.discourse.group/t/contact-analysis-wont-run/1163/20 "2023-10-12T21:34:37Z")
> [@tMKP](#): > > This is the previous result I got from ANSYS. Maximum von-Mises Stress is 1021 MPa required mesh, contact setting, boundary condition, material and load to make it direct comparison with CalculiX model. Previous model did not show large plate, ignoring this interaction may contribute to discrepancy in results. maybe a basic of Ansys mesh (\*.msh) and problem sketch is enough for another user to check. Studying external solver still interesting topics, but the model approach need equally the same, or at least similar.