Postprocessing in abaqus 2

[sunnyqzhang]

Dear all:

I have one 3D contact model with orthotropic material,in which *orientation is used to defined one rectangular local coordinate system. I'd like to view the stress in sort of x' direction which is the linear combination of the stresses of s11 and s33 in global coordinate system. I tried UVARM to define output variable. but it does not work.
Can abaqus viewer define specifical coordinate system to view the stress in any direction? thanks so much!

Sunny Q. Zhang

 

[corus]

You can define a new output variable in Viewer as any mathematical combination of your stored variables, S11, S22 etc. or of a combination of variables from different load steps.

corus

http://www.corusresearch.com

 

[sunnyqzhang]

corus:

Thank you so much. I have a further question then about UVARM. In UVARM, I use GTVERM get variables of "S". and creat two new output variables such as:
...
...
UVARM1=ARRAY(1)*2
UVARM2=ARRAY(1)+ARRAY(2)
...
...
Then in abaqus viewer, I contour these two variables. UVARM1 is exactly twice the amount of S11. but UVARM2 is amount between S11 and S22, where in my case, both S11 and S22 are positive tensile stress. I just wondering, looks like "ARRAY(1)+ARRAY(2)" is not just simple algebra,may be kind of vector adding. i do have no idea about how these results come out. I do appreciate your advice.

 

[corus]

We must be talking about 2 different things here. I'm referring to an option under data manager/create, I think, where you create a new output variable from existing output variables whereby you select the output variable and then the operator, ie. +/-/*/^ etc., followed by further variables, and so on. On Monday I'll check the precise location of this in the tool bar. UVARM and GTVERM I've never heard of unless they're some form of python script.

corus

http://www.corusresearch.com

 

[corus]

I was wrong in my last post. In Viewer go to Tools/create output/fields. In there you can combine your results using various operands so that you can create your new output from a combination of S11 and S33. The new data output will appear under the fields or frames in your comtour options.

corus

http://www.corusresearch.com

 

[sunnyqzhang]

corus:

Sorry bother you again. I tried TOOL->CREAT FIELD OUTPUT, and below output variable, there is one as:

Tag Name Type Description
S1f11_S S Tensor stress component

with many operators right side. My problem is, I cannot get stress component out, I mean, cannot get S11, S22 et. and combine with the operater. I checked related example, and only find one like: S1f2_s-S1f1_s, which is also not deal with component. Can you give some detail? Thank you!

 

[corus]

I've not heard of S1f11_S but generally if you include S in your *El field output, or just leave the preset values, then you should see all the components, S11, S22, S33 etc., just as you would if you selected the field variable for contouring.
If I remember you simply click or type in the variable and then click on the operand. These should appear in a separate line in the box so you can see the operation you're carrying out.
Which element are you using and what did you use in your *El field data line?
I take it that UVARM is some sort of User Subroutine, which I'm not familiar with.

corus

http://www.corusresearch.com

 

[sunnyqzhang]

The element type is C3D6 and C3D8, a simple indentation contact model. Actually, in RESULT->FIELD OUTPUT, I can see S11,S22 et. But in TOOL->CREAT FIELD OUTPUT, I can only see S1f11_s, in which "1" means step 1, "11"means frame 11 (similarly s1f11_u for displacemt). And if I just select S1f11_s as the created field output, I can contour in RESULT->FIELD OUTPUT its components of S11,et. I'd like to creat one field variable as: s11*cos(t)^2+s33*sin(t)^2-2*s13*cos(t)*sin(t). But there is no field variables like S1f11_S11 et. for me to select and organize. Do you think I miss some operation?

 

[corus]

I was totally wrong with the Viewer idea. You're right, you can't do a thing with the create field output other than manipulate the whole of the stress tensor. What a load of @#@!*!

With the UVARM you are working on stresses at the element integration points but plotting rsults at the nodal positions. Are you sure that nodal averaging hasn't in some way given you a different value to the one you were expecting? If you create UVARMs for ARRAY(1) and ARRAY(2) separately and print them out with *el print, then you could check to see if the additive operation is working or is in fact some kind of vector addition, as you first said.


corus

http://www.corusresearch.com

 

[sunnyqzhang]

In UVARM, results will be plotted at nodal position? I thought the integration points are the default choice, it is nice to double check it.I am thinking using matlab to contour it after getting data from .dat file with setting el. print at nodal position. But it is quite time consuming.

 

[corus]

Element stresses are printed at the integration points by default. In Viewer though the contours are based upon nodal results. These are extrapolated from the integration points and then averaged between elements. Modify the nodal averaging value in the results/options from 75% down to 0 and you'll see a patchwork stress pattern, which presumably is the element stresses rather than the nodal averaged stresses. This works best when there is only a single integration point.

corus

http://www.corusresearch.com