# 3D Rigid bar element **URL:** \ **Category:** Uncategorized\ **Created:** [October 15, 2020, 12:00pm UTC](https://calculix.discourse.group/t/3d-rigid-bar-element/258 "2020-10-15T12:00:19Z")\ **Posts on this page:** 7\ **Page:** 1
**Author:** ![carlomontec](https://avatars.discourse-cdn.com/v4/letter/c/7c8e57/32.png) [@carlomontec](https://calculix.discourse.group/u/carlomontec)\ **Post date:** [October 15, 2020, 12:00pm UTC](https://calculix.discourse.group/t/3d-rigid-bar-element/258/1 "2020-10-15T12:00:19Z")
Hello, does someone knows how to create a rigid bar element in CCX? I need to set a point mass and connect it to the main FE structure via rigid element(s). The idea is to capture the inertia effects of a small body (point mass) in a modal analysis of a big structure. The added mass has no effects in terms of stiffness. I placed a point mass in a node at the center of gravity of the small body, but I dont know how to connect it to the main structure. If I remember correctly, in NASTRAN the RBE3 would be a good solution. I am not sure if I can replicate it in CCX. I thought of using translation equations. One complication I thought is that we expect torsion of the main structure, so the translation of one node of the main structure wont replicate the rotation of the small rigid body. I also thought I could set 3 beams with zero mass and almost infinite stiffness in an triangular arrangement. Greetings, Carlo ---
**Author:** ![SergioP](https://yyz2.discourse-cdn.com/free1/user_avatar/calculix.discourse.group/sergiop/32/10_2.png) [@SergioP](https://calculix.discourse.group/u/SergioP)\ **Post date:** [October 15, 2020, 12:50pm UTC](https://calculix.discourse.group/t/3d-rigid-bar-element/258/2 "2020-10-15T12:50:06Z")
You could try with \*RIGID BODY card. ---
**Author:** ![xyont](https://yyz2.discourse-cdn.com/free1/user_avatar/calculix.discourse.group/xyont/32/3553_2.png) [@xyont](https://calculix.discourse.group/u/xyont)\ **Post date:** [October 16, 2020, 3:55am UTC](https://calculix.discourse.group/t/3d-rigid-bar-element/258/3 "2020-10-16T03:55:36Z")
hi, as i know **RBE3** in Nastran is different compared to \ ***Rigid Body** keywords in CalculiX or Abaqus, it has an option to avoid over-constrained condition (e.g stay plane as is as undeformed, poison effect, warping in steel column modeling as solid with concentrated force/moment). you can use \ ***Coupling** keywords to modeling similar conditions and set DOF’s you may consider to constrained/activated. previously i was took some comparison for simple case ([links](http://syont.blogspot.com/2018/02/distribusi-beban-terkonsentrasi-ke.html)). non-english writen so language translation is required, but did many pictures from screenshot can speak itself? thank you, ---
**Author:** ![vicmw](https://avatars.discourse-cdn.com/v4/letter/v/6de8d8/32.png) [@vicmw](https://calculix.discourse.group/u/vicmw)\ **Post date:** [October 16, 2020, 7:37am UTC](https://calculix.discourse.group/t/3d-rigid-bar-element/258/4 "2020-10-16T07:37:51Z")
Just adding to what xyont said, \*COUPLING with \*DISTRIBUTING is like RBE3. I have used it with a point mass before. But it’s more finnicky than \*RIGID BODY so avoid doing anything fancy. It can fail or produce wrong results if you have very large rotations (\>~10 degrees), try to couple rotational DOFs, or use \*TRANSFORM on it sometimes even though it’s OK other times. ---
**Author:** ![xyont](https://yyz2.discourse-cdn.com/free1/user_avatar/calculix.discourse.group/xyont/32/3553_2.png) [@xyont](https://calculix.discourse.group/u/xyont)\ **Post date:** [October 16, 2020, 8:58am UTC](https://calculix.discourse.group/t/3d-rigid-bar-element/258/5 "2020-10-16T08:58:06Z")
hi **vicmw** , thanks for add some hint. i did not look into specific details, only want to says similarity between Nastran and Calculix in RBE3. is failure problem comes from \*COUPLING with \*DISTRIBUTING keywords only? how about DCOUP3D element. any simple examples are worth of me to learn. thank you, ---
**Author:** ![vicmw](https://avatars.discourse-cdn.com/v4/letter/v/6de8d8/32.png) [@vicmw](https://calculix.discourse.group/u/vicmw)\ **Post date:** [October 16, 2020, 10:22am UTC](https://calculix.discourse.group/t/3d-rigid-bar-element/258/6 "2020-10-16T10:22:51Z")
I made a mistake, sorry. You can’t use \*DISTRIBUTING for this because it neglects the offset of the reference node from the mesh it’s connected to. Also, I’m having trouble getting it to work with \*FREQUENCY. @carlomontec, I think you have to use either: - \*RIGID BODY which rigidly connects all its nodes. - \*COUPLING with \*KINEMATIC which behaves like \*RIGID BODY. - Write constraint equations yourself to couple all the DOFs. Yuck. - Beam elements with high stiffness. - \*DISTRIBUTING COUPLING maybe. See below. @xyont, I don’t have much experience with DCOUP3D and \*DISTRIBUTING COUPLING except that it seems to be more low-level than \*COUPLING and you have to specify the weights yourself which would be tricky on an unstructured mesh. Hopefully someone else can add more. ---
**Author:** ![carlomontec](https://avatars.discourse-cdn.com/v4/letter/c/7c8e57/32.png) [@carlomontec](https://calculix.discourse.group/u/carlomontec)\ **Post date:** [October 23, 2020, 4:17pm UTC](https://calculix.discourse.group/t/3d-rigid-bar-element/258/7 "2020-10-23T16:17:50Z")
Thank you all for your valuable contributions.