# Error when reading \*KINEMATIC COUPLING **URL:** \ **Category:** Uncategorized\ **Created:** [October 8, 2023, 9:06am UTC](https://calculix.discourse.group/t/error-when-reading-kinematic-coupling/1864 "2023-10-08T09:06:18Z")\ **Posts on this page:** 12\ **Page:** 1
**Author:** ![Nils](https://avatars.discourse-cdn.com/v4/letter/n/d6d6ee/32.png) [@Nils](https://calculix.discourse.group/u/Nils)\ **Post date:** [October 8, 2023, 9:06am UTC](https://calculix.discourse.group/t/error-when-reading-kinematic-coupling/1864/1 "2023-10-08T09:06:19Z")
Hello! I’m a calculix first timer and applying CL32-win32bit on a simple structural mechanics problem. There are 4 screws, which I model with a simple coupling spider: \*KINEMATIC COUPLING, REF NODE=356 Screw\_1, 1, 3 \*KINEMATIC COUPLING, REF NODE=357 Screw\_2, 1, 3 \*KINEMATIC COUPLING, REF NODE=17533 Screw\_3, 1, 3 \*KINEMATIC COUPLING, REF NODE=17550 Screw\_4, 1, 3 The sets “Screw\_\*” contain the nodes of the washer elements of parts to be joined. The error message is \*ERROR reading \*BOUNDARY. Card image: Srew\_1,1,3 If someone has suggestions how this problem emerges and how to solve, I’d be very thankful! Best Regards Nils ---
**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\ **Post date:** [October 8, 2023, 9:38am UTC](https://calculix.discourse.group/t/error-when-reading-kinematic-coupling/1864/2 "2023-10-08T09:38:59Z")
If a boundary condition is defined within a step, it should use this format: ```auto *BOUNDARY node_set, first_DOF, last_DOF, value ``` So it should be: ```auto *BOUNDARY Screw_1, 1, 3, 0 ``` if you want to fix those DOFs. ---
**Author:** ![Nils](https://avatars.discourse-cdn.com/v4/letter/n/d6d6ee/32.png) [@Nils](https://calculix.discourse.group/u/Nils)\ **Post date:** [October 8, 2023, 10:07am UTC](https://calculix.discourse.group/t/error-when-reading-kinematic-coupling/1864/3 "2023-10-08T10:07:03Z")
Thanks Calc\_em. I think the error message is a little misleading, because the error seems to be in the coupling definition and there is the value that you are talking about not required. I have no idea why “\*Boundary” is printed in the error message 🤔 My boundary is defined exactly as you wrote. I was already modifying several things using couplings, but somehow this seems not straight forward coming from abaqus ---
**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\ **Post date:** [October 8, 2023, 10:37am UTC](https://calculix.discourse.group/t/error-when-reading-kinematic-coupling/1864/4 "2023-10-08T10:37:59Z")
Actually, the kinematic coupling definition in CalculiX should look like this: ```auto *COUPLING, REF NODE=..., SURFACE=..., CONSTRAINT NAME=... *KINEMATIC first_DOF, last_DOF ``` Calculix doesn’t have the `*KINEMATIC COUPLING` keyword. ---
**Author:** ![Nils](https://avatars.discourse-cdn.com/v4/letter/n/d6d6ee/32.png) [@Nils](https://calculix.discourse.group/u/Nils)\ **Post date:** [October 8, 2023, 4:17pm UTC](https://calculix.discourse.group/t/error-when-reading-kinematic-coupling/1864/5 "2023-10-08T16:17:18Z")
Thank you again Calc\_em. I tried now to work with a Coupling Type Kinematic. Below you find both Coupling and surface definition \*SURFACE, NAME=Screw\_1, TYPE=NODE Screw\_1, 1. \*COUPLING, CONSTRAINT NAME=COUPLING\_114, REF NODE=356, SURFACE=Screw\_1 \*KINEMATIC 1, 6 and I still get an error message \*ERROR reading \*SURFACE: only one entry per line allowed \*ERROR reading \*SURFACE. Card image: Screw\_1,1. Can you tell, what is the error now? Thanks in advance for your reply! ---
**Author:** ![jbr](https://avatars.discourse-cdn.com/v4/letter/j/ecccb3/32.png) [@jbr](https://calculix.discourse.group/u/jbr)\ **Post date:** [October 8, 2023, 4:38pm UTC](https://calculix.discourse.group/t/error-when-reading-kinematic-coupling/1864/6 "2023-10-08T16:38:16Z")
@Nils I believe you need to use: ```auto *SURFACE, NAME=SurfName, TYPE=ELEMENT ElementID, FaceID ``` then ```auto *COUPLING, CONSTRAINT NAME=Coup_Name, REF NODE=ID_1, SURFACE=SurfName *KINEMATIC 1, 6 ``` ElementID can be replaced with an element set. Are you using any particular pre-processor? Can you send the input deck to debug it? ---
**Author:** ![Nils](https://avatars.discourse-cdn.com/v4/letter/n/d6d6ee/32.png) [@Nils](https://calculix.discourse.group/u/Nils)\ **Post date:** [October 8, 2023, 5:29pm UTC](https://calculix.discourse.group/t/error-when-reading-kinematic-coupling/1864/7 "2023-10-08T17:29:26Z")
Thanks for your answer and offer! I’ll try to debug and then get back to you! ---
**Author:** ![Disla](https://yyz2.discourse-cdn.com/free1/user_avatar/calculix.discourse.group/disla/32/3548_2.png) [@Disla](https://calculix.discourse.group/u/Disla)\ **Post date:** [October 9, 2023, 6:22am UTC](https://calculix.discourse.group/t/error-when-reading-kinematic-coupling/1864/8 "2023-10-09T06:22:13Z")
Hi, I thought kinematic coupling was only allowed for degrees of freedom from 1 to 3. ¿¿?? Manual says two times (only 1, 2 or 3 allowed). Regards ---
**Author:** ![jbr](https://avatars.discourse-cdn.com/v4/letter/j/ecccb3/32.png) [@jbr](https://calculix.discourse.group/u/jbr)\ **Post date:** [October 9, 2023, 6:15pm UTC](https://calculix.discourse.group/t/error-when-reading-kinematic-coupling/1864/9 "2023-10-09T18:15:24Z")
> [@Disla](#): > > Manual says two times (only 1, 2 or 3 allowed). That is correct. My bad, I Crtl+v too fast and did not change the limits. No rotational DOFs. ---
**Author:** ![Disla](https://yyz2.discourse-cdn.com/free1/user_avatar/calculix.discourse.group/disla/32/3548_2.png) [@Disla](https://calculix.discourse.group/u/Disla)\ **Post date:** [October 9, 2023, 8:51pm UTC](https://calculix.discourse.group/t/error-when-reading-kinematic-coupling/1864/10 "2023-10-09T20:51:52Z")
This approach it is kind of weird with its surface definition through the nodes , but it is the only kinematic combination that works with shells for me. Yours: \*SURFACE, NAME=Screw\_1, TYPE=NODE Screw\_1, 1. \*COUPLING, CONSTRAINT NAME=COUPLING\_114, REF NODE=356, SURFACE=Screw\_1 \*KINEMATIC 1, 6 Try this: \*SURFACE,NAME=Screw\_1,TYPE=NODE Screw\_1 \*COUPLING,REF NODE=356,SURFACE=Screw\_1,CONSTRAINT NAME=COUPLING\_114 \*KINEMATIC 1,3 ---
**Author:** ![huangsx](https://avatars.discourse-cdn.com/v4/letter/h/53a042/32.png) [@huangsx](https://calculix.discourse.group/u/huangsx)\ **Post date:** [June 19, 2024, 11:54pm UTC](https://calculix.discourse.group/t/error-when-reading-kinematic-coupling/1864/11 "2024-06-19T23:54:11Z")
Hi, Disla Do you have any ideas about using kinematic coupling with rotational DOFs? It looks strange only with translational DOFs. Thank you. ---
**Author:** ![Disla](https://yyz2.discourse-cdn.com/free1/user_avatar/calculix.discourse.group/disla/32/3548_2.png) [@Disla](https://calculix.discourse.group/u/Disla)\ **Post date:** [June 20, 2024, 7:28am UTC](https://calculix.discourse.group/t/error-when-reading-kinematic-coupling/1864/12 "2024-06-20T07:28:36Z")
Not with Kinematic card. That is a limitation of ccx. If you don’t mind some model stiffening you could try defining two rigid bodies sharing a commond ROT. ![imagen](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/4/468a6ddef6ec9162a099844ebb52859f528f6923.png)