Why CPE6 has 9 integration points

Hi all,

In my understanding, CPE6 element should only has 3 integration points. However, when I try to print information on the integration points of one CPE6 element using following command:

*EL PRINT, ELSET = Element_Set-1, FREQUENCY = 10000

And get the following dat file,

                    S T E P       1

                            INCREMENT    15

total force (fx,fy,fz) for set FOOTING and time 0.1000000E+01

   -2.541947E+00 -2.728767E+01  3.156364E-13

stresses (elem, integ.pnt.,sxx,syy,szz,sxy,sxz,syz) for set ELEMENT_SET-1 and time 0.1000000E+01

   772   1 -3.134375E-02 -4.168847E-02 -3.650972E-02  8.558429E-03 -3.000474E-16  4.910472E-15
   772   2 -1.898157E-02 -2.876880E-02 -2.387324E-02  8.720810E-03  3.676036E-15 -8.110479E-16
   772   3 -3.039993E-02 -4.111506E-02 -3.574695E-02  8.443721E-03  6.359709E-16 -1.281660E-14
   772   4 -3.134375E-02 -4.168847E-02 -3.650972E-02  8.558429E-03 -9.571245E-16 -8.933567E-16
   772   5 -1.898157E-02 -2.876880E-02 -2.387324E-02  8.720810E-03 -1.100504E-15  6.909238E-16
   772   6 -3.039993E-02 -4.111506E-02 -3.574695E-02  8.443721E-03  2.415343E-16  6.398212E-16
   772   7 -3.134375E-02 -4.168847E-02 -3.650972E-02  8.558429E-03 -4.695136E-15  1.653942E-14
   772   8 -1.898157E-02 -2.876880E-02 -2.387324E-02  8.720810E-03 -9.173169E-15 -1.845234E-14
   772   9 -3.039993E-02 -4.111506E-02 -3.574695E-02  8.443721E-03  1.298908E-14 -9.895379E-15

global coordinates (elem, integ.pnt.,x,y,z) for set ELEMENT_SET-1 and time 0.1000000E+01

   772   1  3.474444E+02 -6.239917E+02 -3.872983E-01
   772   2  3.892147E+02 -5.995540E+02 -3.872983E-01
   772   3  3.478147E+02 -5.744767E+02 -3.872983E-01
   772   4  3.474444E+02 -6.239917E+02  0.000000E+00
   772   5  3.892147E+02 -5.995540E+02  2.081668E-17
   772   6  3.478147E+02 -5.744767E+02  0.000000E+00
   772   7  3.474444E+02 -6.239917E+02  3.872983E-01
   772   8  3.892147E+02 -5.995540E+02  3.872983E-01
   772   9  3.478147E+02 -5.744767E+02  3.872983E-01

Among these 9 integration points, 3 points have a z coordinate of -3.872983E-01 and another 3 points have a z coordinate of -3.872983E-01.

I assume the reason is I use 1 mm in the *solid section:

*Solid section, Elset=Internal_Selection-1_Solid_Section-1, Material=Material-1

It seems that this CPE6 element has 9 integration points. That makes me confused.

Kind regards,

@Ran.Tu , CPE6 is expanded in both local z-direction out to a wedge element as described in the CCX manual. The C3D15 wedge element is with 9 integration points.


Hi fgr,

Thanks for your reply. That makes sense. And I also read secition 6.2.26 of ccx manual.

Now my understanding is plane strain element is actually expanded to 3D element when ccx conduction calculation. And based on ccx manual, the displacement in z-direction of all nodes (not only the mid-nodes) is zero.

Now, I am concerned that:

  1. If I employ a subroutine for performing operations at integration points, such as utilizing sigini.f to set initial stress or using umat to define custom material properties, Am I actually conducting these operations at the integration points of a 2D plane strain element or a 3D extended element?

  2. When I use *EL, PRINT to print information at integration points, is it possible to only print information at integration points on mid-plane (where z = 0 for plane strain element)? As I found that information at integration points on mid-plane is adequate.

Kind regard,

maybe it helps if your use output=2D


Hi dichtstoff,

I have a try on my model by using:


But in the printed dat file, I still get stress at all 9 integration points for the extended 3D elements.

And I checked the ccx manual, for *NODE FILE of plane element, the default parameter is OUTPUT=2D.

And based on the manual, even for *EL FILE, the default parameter is also OUTPUT=2D for plane strain element.

However, *EL PRINT has no parameter of OUTPUT. So I do not know if it is possible to only print information at integration points on mid-plane.

Kind regards,

When you’re asking so specific questions about the CPE6 expansion to wedge element I’m not able to give you the answer since I haven’t used of analyzed this issue maybe other users inside here can give you specific answers otherwise you will need to analyze the code by youself

Not possible using the standard interface, you should modify the source code. However as you have noticed for stresses the first 3 points, the second 3 points and the third 3 point provide same data as should be for a plane stress element, szz !=0, and ezz=0 always. So whatever you intend to do you only have to consider that data but when transferring data with ccx consider you have to triple it. As .dat is a formatted file you can optimize the reading for sure.

On the other hand internally only 3D exist so I’d use 9 integration points.

Thank you JuanP74. That makes sense.