nblock in VUMAT

[brunda]

Hello all,

I am working on polymer constitutive modeling and have recently started using ABAQUS.

I am currently using VUMAT for defining my user material. I am confused as to what 'nblock' refers to.

The manuals say that it is the number of material points. Are these equal to number of elements? or are these similar to guass points. And how does abaqus decides the value for nblock.

Also, is there a way to get the element number in vumat subroutine?

Any help is much appreciated.

regards
B

[Kumar Kurambakurash]

Hi,

'nblock' refers to the ID of the Gauss pt among stacked (or vectorized) Gauss pts.

And yes, there are ways to get the element number.
One attractive method is using a ghost shell function.

Kumar

[brunda]

Hi Kumar,

Thanks for your reply...

I use C3D8R elements and I gathered from internet that C3D8R has only one integration point. Is that the gauss point?

Also, when I print the nblock to output file, I see the value as always equal to the number of elements.

Am I missing something very basic? Also I have tried checking for the ghost shell function, but didnt find much information.. Could you please elaborate on it.

Thanks again
B

[Kumar Kurambakurash]

You are using C3D8R elements which means continuum 3D 8 noded reduced integration. A reduced integration of this kind has a single Gauss pt.
Thats why you have matching GP and element numbers.

Regarding the second, apply the following cover,

subroutine vumat (
c Read only -
1 jblock, ndir, nshr, nstatev, nfieldv, nprops, lanneal,
2 stepTime, totalTime, dt, cmname, coordMp, charLength,
3 props, density, strainInc, relSpinInc,
4 tempOld, stretchOld, defgradOld, fieldOld,
5 stressOld, stateOld, enerInternOld, enerInelasOld,
6 tempNew, stretchNew, defgradNew, fieldNew,
c Write only -
7 stressNew, stateNew, enerInternNew, enerInelasNew )
c
include 'vaba_param.inc'
c
dimension jblock(*), props(nprops),density(*), coordMp(*),
1 charLength(*), strainInc(*),
2 relSpinInc(*), tempOld(*),
3 stretchOld(*),
4 defgradOld(*),
5 fieldOld(*), stressOld(*),
6 stateOld(*), enerInternOld(*),
7 enerInelasOld(*), tempNew(*),
8 stretchNew(*),
9 defgradNew(*),
1 fieldNew(*),
2 stressNew(*), stateNew(*),
3 enerInternNew(*), enerInelasNew(*)
c
character*80 cmname

parameter (
1 i_umt_nblock = 1,
2 i_umt_npt = 2,
3 i_umt_layer = 3,
4 i_umt_kspt = 4,
5 i_umt_noel = 5 )

call vumatXtrArg ( jblock(i_umt_nblock),
1 ndir, nshr, nstatev, nfieldv, nprops, lanneal,
2 stepTime, totalTime, dt, cmname, coordMp, charLength,
3 props, density, strainInc, relSpinInc,
4 tempOld, stretchOld, defgradOld, fieldOld,
5 stressOld, stateOld, enerInternOld, enerInelasOld,
6 tempNew, stretchNew, defgradNew, fieldNew,
7 stressNew, stateNew, enerInternNew, enerInelasNew,
8 jblock(i_umt_noel), jblock(i_umt_npt),
9 jblock(i_umt_layer), jblock(i_umt_kspt))

return
end

c ----------------------------------------------------------------------------------

subroutine vumatXtrArg (
c read only -
1 nblock, ndir, nshr, nstatev, nfieldv, nprops, lanneal,
2 stepTime, totalTime, timeinc, cmname, coordMp, charLength,
3 props, density, strainInc, relSpinInc,
4 tempOld, stretchOld, defgradOld, fieldOld,
3 stressOld, stateOld, enerInternOld, enerInelasOld,
6 tempNew, stretchNew, defgradNew, fieldNew,
c write only -
5 stressNew, stateNew, enerInternNew, enerInelasNew,
c read only extra arguments -
6 nElement, nMatPoint, nLayer, nSecPoint)
c
include 'vaba_param.inc'
c
c all arrays dimensioned by (*) are not used in this algorithm
dimension props(nprops), density(nblock),
1 strainInc(nblock,ndir+nshr),
2 relSpinInc(nblock,nshr), defgradOld(nblock,9),
4 stressOld(nblock,ndir+nshr),
5 stateOld(nblock,nstatev), enerInternOld(nblock),
6 enerInelasOld(nblock),
7 stretchNew(nblock,ndir+nshr), defgradNew(nblock,9),
8 stressNew(nblock,ndir+nshr)

dimension enerInelasNew(nblock),stateNew(nblock,nstatev),
1 enerInternNew(nblock)

dimension nElement(nblock),nMatPoint(nblock),nLayer(nblock),
1 nSecPoint(nblock)

character*80 cmname


c make computations for every material point
c -----------------------------------------------------------------------

do 1000 nblck = 1,nblock

Nelem=nElement(nblck) ! here we go
blah blah blah

enddo

return
end

[brunda]

thanks again.. things are much clearer now...

regards

[Jorgen]

Hi Kumar,

You are presenting some very interesting information

I did not know you could determine the element number from within a VUMAT subroutine. How on earth did you figure that out

I assume that you have tried that approach and that it works, is that right? Is your approach a known feature? Are you working for Abaqus (Simulia)?

Very cool stuff!
Jorgen

[Kumar Kurambakurash]

Dear Jorgen,

It really is cool I agree.

I remember finding the method through a long web search.

Thus the credit is not mine.

However I have tried the method and it works perfectly fine and and it is reliable.

Best

Kumar

[Kumar Kurambakurash]

Hi Kumar,

Thanks for your reply...

I use C3D8R elements and I gathered from internet that C3D8R has only one integration point. Is that the gauss point?

Also, when I print the nblock to output file, I see the value as always equal to the number of elements.

Am I missing something very basic? Also I have tried checking for the ghost shell function, but didnt find much information.. Could you please elaborate on it.

Thanks again
B

The integration points are called Gauss points since the required integrations follow Gaussian quadrature.

[Andrew Litchfield]

Hi guys,

I light of the above comments, I also had a question regarding nblock. I have been working on a composite laminate damage model in vusdfld (abaqus v6.81) for the initial phase, but will be switching over to vumat soon.

I also need to know the element number at a particular material point when using S4 (four integration points) shell elements with vusdfld. Curiously though when I output nblock for my 196 element model it alternatively displays 136,136......60,60,60 etc

Would anyone have any clues as to why this is? I saved a state variable with the value of "k" every time the subroutine was called, and when checking the value of this variable in Viewer, element 1 corresponds to material pt 1 and element 2, mat pt 2 and so on until I reach element 137 where it starts again with material pt 1.

Any thoughts?

Thanks!
Andrew

[andi]

Hi all,

the V in VUMAT (and all other user defined explicit elements) stands for "vectorized". This means that abaqus passes chunks of data (i.e. nblock elements at once) to the user subroutine for calculation. That's why you always have to loop over nblock: you need to determine the results for all elements abaqus passed to your routine.
For small models, nblock may correspond to the number of elements in your model and subsequently kblock (current increment in nblock) corresponds to the element number. For larger models, there are multiple calls to your subroutine due to performance reasons, hence the number of elements differs from nblock and kblock has to be determined using nElement(kblock) (as mentioned before)...

Regards

Andi