See attached

You can obtain the position of the integration points by using output variable COORD.

Thanks Henry, could you be a bit more specific? I couldn’t find the COORD variable.

You need to write it out as field output request, it is not done by default,

See attached

Thanks Muntaseer. It really helped!

Hi everyone, I have the same question but for a user element. I am using a 4 noded quad with a 2 X 2 gauss integration.

Dear Nothando Mhlongo ,

I suppose you know that the position of Gauss points is usually defined within the user element. However, this is done with respect to the element coordinate system such that problems might arise if you'd like to obtain information about all Gauss points in all elements with respect to a global coordinate systems. Are you using ABAQUS and the UEL subroutine? In this case or similar applications, I suggest to introduce so-called ,,dummy'' elements. These elements should already be implemented in your FE code (if you're using ABAQUS, CPS4 might be a good choice, in your case) and are only used for the visualization of results. Since they should not influence the results, their stiffness is set to zero. Please note that it is crucial that the position of the Gauss points is the same in the user element and the dummy elements! You can use these elements to visualize results in contour plots using the GUI. Thus, you can also apply the same procedure as described above to obtain positions of all Gauss points.

If you're using ABQUS and need more information, you're welcome to contact me.

Best regards,

Johanna

Hi everybody,

The question is why do you need to export the coordinates of the Gauß points from Abaqus? If you need them for further post-processing purposes I suggest you just compute them yourselves. From the definition of the finite elements in Abaqus or the User Elements it should be clear where the Gauß points are located in the reference coordinate system (local coordinate system of the master/reference element). These points are compiled in almost every monograph of the finite element method. The global coordinates can then easily be obtained by mapping the local Gauß points to the global coordinate system. This is easily achieved (at least in the isoparametric element concept typically utilized in commercial finite element codes such as Abaqus) by using the shape functions of the finite elements:

xk = Ni(ξk,ηk) Xi

yk = Ni(ξk, ηk)Yi

where (xk,yk) are the global and (ξk,ηk) the local coordinates of the kth Gauß point. (Xi, Yi) denote the global coordinates of the ith node and Ni is corresponding shape function. All these values are known and therefore it is not necessary to extract the Gauß points from Abaqus. The other suggested solutions are all correct and easily implemented for standard elements but seem to be a bit complicated for user elements. From my point of view it would be easiest to just use standard finite element mapping techniques for that purpose.

Best regards

Muntaseer Kainat Hi, Muntaseer, with COORD field output, we can get the nodal coordinate, but is there a way to export the coordinates for the integration point ?

Fei Han As far as I know, there is no way to output the coordinates of integration points directly from Abaqus. One possible solution is to get the COORD at nodal points and hence calculate the integration point coordinates based on associated nodal points.

Wangcheng Zhang Hi, Wangcheng. Thanks for your reply. Good to know, then I'll just let go my trials and write a little matlab code to postprocessing.

If you need them in a file, you can write a UvARM subroutine and then require a dummy user output variable in the analysis. It is very simple because you simply need to open the file in append mode, write COORD array and close the file.

You can find the UVARM structure on manual. You have to add three rows, something like

Open(unit=101, file=‘coords.dat’)

Write(101,*) Noel, NPT, COORDS

Close(101)

you can extract the integration point coordinate in current configuration from the odb file, but before doing it does not forget to add 'COORD' variable in the elemental output request along with the other elemental output variables inside the input file.

*Element Output

COORD

Mayank Chouksey Hi, my impression is COORD will give you nodal coordinates instead of integration point coordinates. Could you confirm?

Hi Fei Han, this is a bit confusing; the variable COORD is unique in that it can be requested for nodal output, element output (i.e., at integration points), or both. Also note that coordinates are current configuration coordinates only if nlgeom=on (I would do some tests just to make sure if this is important to you). Screenshots of descriptions from the documentation are attached.

If both nodal and integration point values are requested, the respective fields can still be extracted and examined separately. Let me know if an example in Python would be helpful. Best of luck to you. -Ken

References:

• Nodal output: Reference Library > Abaqus > Output > Output Variables > Using Abaqus/Standard output variable identifiers > Nodal variables > COORD
• Element output: Reference Library > Abaqus > Output > Output Variables > Using Abaqus/Standard output variable identifiers > Element integration point variables > COORD

Dear Fei Han, thanks to Kenneth I Aycock he has already added the answer.

if you use 'COORD' variable under under 'Node output' you will get the current coordinate of your nodes, but if use it under 'Element output' it will give you the current integration point coordinate. in both the cases NLGOM should be ON.

Thank you, both Kenneth I Aycock and Mayank Chouksey

I think the problem is finally resolved. Let me do a quick summary, since I think many other people (like those who posted here) have the same confusion:

1. In CAE, you can request coordinate outputs by going to the Field Output Request->Edit->Volume/Thickness/Coordinates->COORD, Current nodal coordinates. This way, you will be able to obtain nodal coordinates in ODB, but not the coordinates at the integration points.

2. In order to get the coordinates at the integration points, you'll have to open the input file (***.inp), and add the keyword COORD under Element Output (see figure attached). This cannot be done in CAE as far as I know.

Best,

Fei

Dear Mayank

After completion of analysis, where can we find the requested variables i.e.,, COORD of each integration point.

Thanks and Regards

K Shiva