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
It should be:
*CLOAD
1001,1,10
instead of:
*CLOAD
1001,3,10
because the pre-tension section node uses only the first DOF.
1 Like
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
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:
*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:
*BOUNDARY, FIXED
1001,1,1
This way you can apply the actual load to the part.
1 Like
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:
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
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
1 Like
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:
wbr dichtstff
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.
1 Like
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
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.