FEAP User Forum
FEAP => Input File Issues => Topic started by: halleluja on June 22, 2021, 02:43:57 AM
-
Hi,
i am trying some cases with contact problem. And use an old code from the forum, see Attachment ico3. In line 57 of the code i try two cases, one with thick,,10 and one wtihout. If i comment out line 57 ! thick,,10, the simulation result looks very strange, see pic1 and the result with thick,,10 see pic2.
I wonder why if i do the simulation without thick, the result is so strange. I think without thick means plain strain.
Best
-
I get an error t hat your blocks are not correctly numbered. This will affect the contact search -- and probably other things too???
-
I get an error t hat your blocks are not correctly numbered. This will affect the contact search -- and probably other things too???
Hi Prof. R.L. Taylor,
thanks a lot for your reply :).
For me there is no error and i got the result as shown in pic2. The version of feap that i used is 8.4.
My problem is that if comment out line 57 thick,,10 and the result is very strange as shown in pic1.
I have just tried the version 8.5. The problem is the same.
-
Run command CHECk your block is left hand rule, not right hand one
-
Hi Prof. R.L. Taylor,
thanks a lot for your advise and the penetration problem is fixed.
I still have a question. if i use material as in input file ico3 mate,1
solid
elas isot 200000 0.3
thick,,10
finite, i get the result shown in pic1. But if instead i use my own element module mate,1
USER,37
20000.0,0.3, where i have developed elmt37.f, it doesn't seems to work as shown in pic2. So my questoin is, if i use my own element, the contact module doesn't work for it?
Best^^
-
The contact module should work just fine with a user element. Thus there must be another problem.
-
I would suggest you first do the frictionless case. Consider the difference between which surface is slave. Study the vertical motion value and how augmenting helps. Also consider use of NEOH as it is more stable. Delete the THICK option -- it multiplies the element thickness by this value, which you probably do not do in the user element - you can adjust penalty parameters to compensate. Once you understand the frictionless case then you can look at frictional behavior.
-
The contact module should work just fine with a user element. Thus there must be another problem.
Yeah, i made a mistake that in my own user element stress 1 is not sigma_xx.
-
I would suggest you first do the frictionless case. Consider the difference between which surface is slave. Study the vertical motion value and how augmenting helps. Also consider use of NEOH as it is more stable. Delete the THICK option -- it multiplies the element thickness by this value, which you probably do not do in the user element - you can adjust penalty parameters to compensate. Once you understand the frictionless case then you can look at frictional behavior.
Dear Prof. R.L. Taylor,
thanks a lot for your advice. The previous errors disappear now. But i still have a question to "CONTact, CHECk". Following is a part code from inputfile ico3neo batch
DT,,dt
loop,time,40
time
! CONTact CHECk
loop,augment,30
LOOP,newton,30
UTANG,,1
NEXT,newton
AUGMent
next,augment
plot,wipe
plot,defo
plot,mesh
plot,stre,1
plot,bound
plot,load
plot,pair,1,2
next,time
endThe output will be a little different if i comment out "CONTact, CHECk". Could you explain it please? And can you take a look of my inputfile ico3neo from line 110 to line 131 in attachment, which is my the solution strategy? Did i use the augmented lagrangian method correctly?
-
Contact CHECK sets a contact state that does not change due into solution iteration. You should loop around the check a few times.
Without CHECK the contact state is checked every iteration during solution.
-
Contact CHECK sets a contact state that does not change due into solution iteration. You should loop around the check a few times.
Without CHECK the contact state is checked every iteration during solution.
Dear Prof. R.L. Taylor,
thanks a lot for your reply. So if i have a solution strategy for my contact problem as
batch
DT,,dt
loop,time,40
time
loop,augment,3
LOOP,newton,30
UTANG,,1
NEXT,newton
AUGMent
next,augment
next,time
endIt is without "Contact CHECK", so it should be equivalent
batch
DT,,dt
loop,time,40
time
loop,augment,3
LOOP,newton,30
CONTact CHECk ！！！！！！！！！！！
UTANG,,1
NEXT,newton
AUGMent
next,augment
next,time
endBut for my contact problem, there is still a difference between two solution strategies as shown in attachment.
-
This depends on what you want to do, but often people fix the contact, iterate to convergence and then re-check the contact. Something like:
loop,,3
contact check
loop,,10
tang,,1
next
next