# Beam Elements with Volumetric Elements **URL:** \ **Category:** Uncategorized\ **Created:** [April 3, 2023, 1:13pm UTC](https://calculix.discourse.group/t/beam-elements-with-volumetric-elements/1574 "2023-04-03T13:13:41Z")\ **Posts on this page:** 14\ **Page:** 1
**Author:** ![calc4fem](https://avatars.discourse-cdn.com/v4/letter/c/3da27b/32.png) [@calc4fem](https://calculix.discourse.group/u/calc4fem)\ **Post date:** [April 3, 2023, 1:13pm UTC](https://calculix.discourse.group/t/beam-elements-with-volumetric-elements/1574/1 "2023-04-03T13:13:41Z")
When solving typical task, such as structure with bolts, I can’t determine stress in the beam elements. When running inp file at pre-processor, I can see beam elements in the mode. When starting .frd, beams are disappear. \*EL PRINT is not working for beams. The example: pret3.inp, all versions. How I can solve it? ---
**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:** [April 3, 2023, 1:24pm UTC](https://calculix.discourse.group/t/beam-elements-with-volumetric-elements/1574/2 "2023-04-03T13:24:12Z")
> [@calc4fem](#): > > When starting .frd, beams are disappear. \*EL PRINT is not working for beams. CalculiX CrunchiX User’s Manual → \*PRE-TENSION SECTION: > For beam elements a linear multiple point constraint is created between the nodes belonging to the beam element. The beam element itself is deleted,i.e. it will not show up in the frd-file. Therefore, no other boundary conditions or loads can be applied to such elements. Their only reason of existence is to create an easy means in which the user can define a pretension. ---
**Author:** ![calc4fem](https://avatars.discourse-cdn.com/v4/letter/c/3da27b/32.png) [@calc4fem](https://calculix.discourse.group/u/calc4fem)\ **Post date:** [April 3, 2023, 2:13pm UTC](https://calculix.discourse.group/t/beam-elements-with-volumetric-elements/1574/3 "2023-04-03T14:13:36Z")
Thank you. But bolt force is the main result in this case. How I can get it for deleted element? пн, 3 апр. 2023 г., 17:34 Calc\_em via CalculiX \<[notifications@calculix.discoursemail.com](mailto:notifications@calculix.discoursemail.com)\>: ---
**Author:** ![JuanP74](https://avatars.discourse-cdn.com/v4/letter/j/b5a626/32.png) [@JuanP74](https://calculix.discourse.group/u/JuanP74)\ **Post date:** [April 3, 2023, 2:29pm UTC](https://calculix.discourse.group/t/beam-elements-with-volumetric-elements/1574/4 "2023-04-03T14:29:31Z")
try `read pret3.inp nam` in the terminal after loading .frd however you need to create results for the elements using \*EL FILE or \*ELEMENT OUTPUT. Otherwise check your results at pret3.dat file. Do not forget the different behavior of beams when using parameter OUTPUT=3D (default) or OUTPUT=2D. ---
**Author:** ![calc4fem](https://avatars.discourse-cdn.com/v4/letter/c/3da27b/32.png) [@calc4fem](https://calculix.discourse.group/u/calc4fem)\ **Post date:** [April 3, 2023, 5:42pm UTC](https://calculix.discourse.group/t/beam-elements-with-volumetric-elements/1574/5 "2023-04-03T17:42:08Z")
Thank you, but beam results are stay zero at frd or dat. ---
**Author:** ![JuanP74](https://avatars.discourse-cdn.com/v4/letter/j/b5a626/32.png) [@JuanP74](https://calculix.discourse.group/u/JuanP74)\ **Post date:** [April 3, 2023, 6:24pm UTC](https://calculix.discourse.group/t/beam-elements-with-volumetric-elements/1574/6 "2023-04-03T18:24:42Z")
you have to request them; in `pret3` example they’re not requested. the `pret3` input deck part requesting output follows: > \*STEP > \*STATIC > \*CLOAD > 99,1,1. > \*NODE PRINT,NSET=Nall > U > \*NODE PRINT,NSET=Ncoup1,TOTALS=YES > RF > \*NODE PRINT,NSET=Ncoup2,TOTALS=YES > RF > \*END STEP you have to request stresses or whatever you need, from all elements or the beam elements in particular. ---
**Author:** ![calc4fem](https://avatars.discourse-cdn.com/v4/letter/c/3da27b/32.png) [@calc4fem](https://calculix.discourse.group/u/calc4fem)\ **Post date:** [April 3, 2023, 6:48pm UTC](https://calculix.discourse.group/t/beam-elements-with-volumetric-elements/1574/7 "2023-04-03T18:48:35Z")
Hello Juan, I mean, there are no results for beam at .frd file, as well as beams are eliminated When you read/add inp, you are not obtaining results, just adding input to output But \*NODE PRINT,NSET=Ncoup1,TOTALS=YES RF \*NODE PRINT,NSET=Ncoup2,TOTALS=YES RF may be the answer. If I can get forces at the ends of bolt, the problem is solved Regards ---
**Author:** ![JuanP74](https://avatars.discourse-cdn.com/v4/letter/j/b5a626/32.png) [@JuanP74](https://calculix.discourse.group/u/JuanP74)\ **Post date:** [April 3, 2023, 8:30pm UTC](https://calculix.discourse.group/t/beam-elements-with-volumetric-elements/1574/8 "2023-04-03T20:30:08Z")
OK. now I see what you mean, my mistake. According to the manual: > Internally, the nodes belonging to the element face surface are copied and > a linear multiple point constraint is generated between the nodes expressing > that the mean force is the force specified by the user (or similarly, the mean > differential displacement is the one specified by the user). Therefore, if the > user visualizes the results with CalculiX GraphiX, a gap will be noticed at the > location of the pre-tension section. > For beam elements a linear multiple point constraint is created between the > nodes belonging to the beam element. **The beam element itself is deleted,i.e. > it will not show up in the frd-file**. ---
**Author:** ![calc4fem](https://avatars.discourse-cdn.com/v4/letter/c/3da27b/32.png) [@calc4fem](https://calculix.discourse.group/u/calc4fem)\ **Post date:** [April 3, 2023, 8:30pm UTC](https://calculix.discourse.group/t/beam-elements-with-volumetric-elements/1574/9 "2023-04-03T20:30:09Z")
The other problem, from what I’ve found from calculations, this structure is not really bolted connection. It has certain pretension force between 2 node sets and keeps it constant during loading, what is not completely right. I have to find the way how to keep bolt deformable at all steps, so it is really works as axially preloaded beam between to parts. Regards ---
**Author:** ![calc4fem](https://avatars.discourse-cdn.com/v4/letter/c/3da27b/32.png) [@calc4fem](https://calculix.discourse.group/u/calc4fem)\ **Post date:** [April 3, 2023, 9:07pm UTC](https://calculix.discourse.group/t/beam-elements-with-volumetric-elements/1574/10 "2023-04-03T21:07:30Z")
Hello Juan Probably \*PRE-TENSION card is not the best option because it keeps preload constant at all steps and removing bolt in this case doesn’t mater bolt diameter and material. Is there other option to create preload? Maybe the temperature or some kind of initial strain? ---
**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:** [April 3, 2023, 9:07pm UTC](https://calculix.discourse.group/t/beam-elements-with-volumetric-elements/1574/11 "2023-04-03T21:07:41Z")
> [@calc4fem](#): > > It has certain pretension force between 2 node sets and keeps it > constant during loading, what is not completely right. \*BOUNDARY, FIXED has to be used for that DOF in the second step to freeze preload so that the beam can deform normally due to actual load. At least that’s what needs to be done for 3D solid models of bolts and in software other than CalculiX in which beams are deleted. But you should still be able to apply BCs to the reference node in the second step. ---
**Author:** ![calc4fem](https://avatars.discourse-cdn.com/v4/letter/c/3da27b/32.png) [@calc4fem](https://calculix.discourse.group/u/calc4fem)\ **Post date:** [April 3, 2023, 9:38pm UTC](https://calculix.discourse.group/t/beam-elements-with-volumetric-elements/1574/12 "2023-04-03T21:38:43Z")
Hello, \*BOUNDARY, FIXED should it be applied within 2nd step? how to apply it just to the bolts? ---
**Author:** ![calc4fem](https://avatars.discourse-cdn.com/v4/letter/c/3da27b/32.png) [@calc4fem](https://calculix.discourse.group/u/calc4fem)\ **Post date:** [April 3, 2023, 9:42pm UTC](https://calculix.discourse.group/t/beam-elements-with-volumetric-elements/1574/13 "2023-04-03T21:42:05Z")
For example at the first step I have initial deformation =0.001 \*BOUNDARY 3102,1,1,0.001 does it mean that second step should have \*BOUNDARY,FIXED 3102,1,1, ? ---
**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:** [April 3, 2023, 10:43pm UTC](https://calculix.discourse.group/t/beam-elements-with-volumetric-elements/1574/14 "2023-04-03T22:43:56Z")
Yes, the boundary condition used for pretension in the first step needs to be removed and replaced with a fixed one in the second step.