# \*pre-tension with solid elements **URL:** \ **Category:** Uncategorized\ **Created:** [March 8, 2022, 12:23am UTC](https://calculix.discourse.group/t/pre-tension-with-solid-elements/1025 "2022-03-08T00:23:44Z")\ **Posts on this page:** 10\ **Page:** 1
**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\ **Post date:** [March 8, 2022, 12:23am UTC](https://calculix.discourse.group/t/pre-tension-with-solid-elements/1025/1 "2022-03-08T00:23:44Z")
i have created an example with \*pre-tension according to example pret1.inp. I see see there not really a different, but i get no result!? maybe if someone can have a look into it. if it’s to large,i can downsize it thnx for advance > **[Ihr persönlicher Freigabelink | GMX Cloud](https://c.gmx.net/@324820432001700943/5wktbzccQS24Y2iqYe0ANw)** > > Mit diesem Link erhalten Sie Zugriff auf die mit Ihnen geteilten Daten. ---
**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:** [March 8, 2022, 8:24am UTC](https://calculix.discourse.group/t/pre-tension-with-solid-elements/1025/2 "2022-03-08T08:24:15Z")
It should be: ```auto *CLOAD 1001,1,10 ``` instead of: ```auto *CLOAD 1001,3,10 ``` because the pre-tension section node uses only the first DOF. ---
**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\ **Post date:** [March 8, 2022, 12:04pm UTC](https://calculix.discourse.group/t/pre-tension-with-solid-elements/1025/3 "2022-03-08T12:04:30Z")
hello, thnx a lot for you help. i have now one more question: for my calc. with pre-tension i have to make 2 steps for my calc… so i tried to do these: \*STEP \*STATIC \*CLOAD (pre-tension) 1001,1,10 \*END STEP \*STEP \*STATIC \*CLOAD (pre-tension) 1001,1,-10 \*END STEP and the result should be zero, but these is not working!? wbr ---
**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:** [March 8, 2022, 12:51pm UTC](https://calculix.discourse.group/t/pre-tension-with-solid-elements/1025/4 "2022-03-08T12:51:31Z")
It works. You will see this if you apply large deformation scale factor (e.g. 2000). You can also request the history output for the pre-tension section node: ```auto *NODE PRINT, NSET=Npretension U ``` The result will be: - end of step 1: U1 = 0.0004673933 - end of step 2: U1 = -0.0004673933 Don’t trust color maps in the case of pre-tension, they can be very misleading. By the way, the usual approach in multistep analyses involving pre-tension is to “freeze” it in the second step, using: ```auto *BOUNDARY, FIXED 1001,1,1 ``` This way you can apply the actual load to the part. ---
**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\ **Post date:** [March 8, 2022, 4:22pm UTC](https://calculix.discourse.group/t/pre-tension-with-solid-elements/1025/5 "2022-03-08T16:22:15Z")
thnx, i 'll update it in my calc. so i 'll have three steps? anyway, here is my concept of my (first) implementation. in the next calc. the \*pre-tension card will be included. I hope it is not so worse 🙂 any help, comments and improvements are welcome displacement looks not too bad: ![hcpy_1](https://global.discourse-cdn.com/free1/uploads/calculix/original/1X/9871ee6e914e8c1ebde5aa8936b954b05c1ed161.png) #### temp\_bolt.fbd pnt ! -0.5 -0.5 -2.5 pnt ! 0.5 -0.5 -2.5 pnt ! 0.5 0.5 -2.5 pnt ! -0.5 0.5 -2.5 line ! D001 D002 102 line ! D002 D003 102 line ! D003 D004 102 line ! D004 D001 102 GSUR A001 + SHAPE + L001 + L002 + L003 + L004 seta A001 s A001 swep A001 B001 tra 0 0 5 4 comp B001 u comp B001 u comp B001 d copy B001 B002 tra 0 5 0 elty all he8 mesh all comp A001 d seta A002 s A002 comp A002 d seta A007 s A007 comp A007 d seta A008 s A008 comp A008 d plot n A001 plus n A002 plus n A007 plus n A008 seta bolt se B001 seta stru se B002 seta nodes n bolt enq nodes Ahalfbolt rec \_ \_ 0 del se nodes seta nodes n stru enq nodes Ahalfstru rec \_ \_ 0 del se nodes plus n Ahalfbolt b plus n Ahalfstru g seta D001 p D001 seta D005 p D005 copy D001 refnode\_pt tra 0.5 -0.5 2.5 copy D001 refnode\_01 tra 0.5 0.5 -1.0 copy D005 refnode\_02 tra 0.5 0.5 1.0 seta D009 p D009 seta D00D p D00D copy D009 refnode\_07 tra 0.5 0.5 -1.0 copy D00D refnode\_08 tra 0.5 0.5 1.0 copy D001 rotnode\_01 tra 0.5 3.0 -1.0 copy D005 rotnode\_02 tra 0.5 3.0 1.0 seta refrotnode n refnode\_pt refnode\_01 refnode\_02 seta refrotnode n refnode\_07 refnode\_08 rotnode\_01 seta refrotnode n rotnode\_02 setr all se refrotnode setr bolt se refrotnode setr stru se refrotnode plus na refrotnode s send bolt abq send stru abq send A001 abq nam send A002 abq nam send A007 abq nam send A008 abq nam send Ahalfbolt abq nam send Ahalfstru abq nam send refrotnode abq send refnode\_pt abq nam send refnode\_01 abq nam send refnode\_02 abq nam send refnode\_07 abq nam send refnode\_08 abq nam send rotnode\_01 abq nam send rotnode\_02 abq nam #### temp\_bolt.inp \*HEADING Model: temp\_bolt.inp \*INCLUDE, INPUT=bolt.msh \*INCLUDE, INPUT=stru.msh \*INCLUDE, INPUT=A001.nam \*INCLUDE, INPUT=A002.nam \*INCLUDE, INPUT=A007.nam \*INCLUDE, INPUT=A008.nam \*INCLUDE, INPUT=Ahalfbolt.nam \*INCLUDE, INPUT=Ahalfstru.nam \*INCLUDE, INPUT=refrotnode.msh \*INCLUDE, INPUT=refnode\_pt.nam \*INCLUDE, INPUT=refnode\_01.nam \*INCLUDE, INPUT=refnode\_02.nam \*INCLUDE, INPUT=refnode\_07.nam \*INCLUDE, INPUT=refnode\_08.nam \*INCLUDE, INPUT=rotnode\_01.nam \*INCLUDE, INPUT=rotnode\_02.nam \*RIGID BODY, NSET=NA001, REF NODE=92, ROT NODE=96 \*RIGID BODY, NSET=NA002, REF NODE=93, ROT NODE=97 \*RIGID BODY, NSET=NA007, REF NODE=92, ROT NODE=96 \*RIGID BODY, NSET=NA008, REF NODE=93, ROT NODE=97 \*MATERIAL, Name=steel \*ELASTIC 210000,0.3 \*EXPANSION, ZERO=0 1.2E-5 \*SOLID SECTION, Elset=Ebolt, Material=steel \*SOLID SECTION, Elset=Estru, Material=steel \*INITIAL CONDITIONS,TYPE=TEMPERATURE Nbolt,0 \*STEP \*STATIC \*BOUNDARY \*\*NAhalfbolt,1,3,0 NAhalfstru,3,3,0 Nrefnode\_01,1,2,0 Nrefnode\_02,1,2,0 Nrotnode\_01,1,3,0 Nrotnode\_02,1,3,0 \*TEMPERATURE Nbolt, 1000 \*NODE PRINT, NSET=Nrefnode\_01, TOTALS=ONLY RF, U \*NODE PRINT, NSET=NA001, TOTALS=ONLY RF, U \*NODE PRINT, NSET=NA007, TOTALS=ONLY RF, U \*NODE FILE U \*EL FILE S \*END STEP \*STEP ---
**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:** [March 8, 2022, 6:38pm UTC](https://calculix.discourse.group/t/pre-tension-with-solid-elements/1025/6 "2022-03-08T18:38:20Z")
Two steps should be enough. Usually, it’s done this way: - step 1 - pre-tension - step 2 - fix pre-tension and apply the actual load to which the bolted joint is subjected ---
**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\ **Post date:** [March 8, 2022, 9:34pm UTC](https://calculix.discourse.group/t/pre-tension-with-solid-elements/1025/7 "2022-03-08T21:34:34Z")
i have finished my example, but result is not like in the hand calc.: pre-load is -1000 and external load -500, result should be 1250: i’m not sure about the second step with fix i have freeze it with : ??? \*BOUNDARY 1001,1,0 (1) every help or hint or suggestion is welcome: ![image](https://global.discourse-cdn.com/free1/uploads/calculix/original/1X/dcee6959cb64dae51567f10c0313fe368b185577.png) > **[Ihr persönlicher Freigabelink | GMX Cloud](https://c.gmx.net/@324820432001700943/NT-RUAoVReqCJoDuORwiYg)** > > Mit diesem Link erhalten Sie Zugriff auf die mit Ihnen geteilten Daten. wbr dichtstff ---
**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:** [March 8, 2022, 10:05pm UTC](https://calculix.discourse.group/t/pre-tension-with-solid-elements/1025/8 "2022-03-08T22:05:18Z")
> [@dichtstoff](#): > > i’m not sure about the second step with fix > i have freeze it with : ??? > \*BOUNDARY > 1001,1,0 (1) It should be: > \*BOUNDARY, FIXED > 1001,1,1 Magnitude is not used when the FIXED parameter is included. It freezes the deformation at its state from the previous step. ---
**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\ **Post date:** [March 9, 2022, 8:13pm UTC](https://calculix.discourse.group/t/pre-tension-with-solid-elements/1025/9 "2022-03-09T20:13:11Z")
thnx a lot. it works perfect. these so awesome. I have updated my example file. how is \*PRE-TENSION SECTION card working with beam elements? what have to be replaced with surface? wbr ---
**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:** [March 9, 2022, 9:15pm UTC](https://calculix.discourse.group/t/pre-tension-with-solid-elements/1025/10 "2022-03-09T21:15:30Z")
> [@dichtstoff](#): > > how is \*PRE-TENSION SECTION card working with beam elements? > what have to be replaced with surface? I haven’t tried it with beams yet but, according to the documentation, in such a case the SURFACE parameter has to be replaced with ELEMENT (number of beam element). The rest remains pretty much the same. However, the user’s manual also mentions that the user should keep in mind that the beam element itself is deleted and won’t show up in the frd file. Furthermore, no additional loads or BCs can be applied to it. The nodes of the beam element can be connected with the rest of the model using \*DISTRIBUTING COUPLING.