How to introduce the good thermal conductivities of a tubular composite structure with Ansys ACP ?


I'm trying to make a thermal analysis of composite structure (Pipe "tubular shape"). For this, I need to introduce the orthotropic thermal conductivity values. So, I used homogenisation formulas to get the thermal conductivity of composite Carbon epoxy in the three directions, 

Is my method correct???

someone could give me more information on this subject.

Thank you,


  • sharveysharvey San Diego, CAMember
    edited September 18


    Yes, you can use thermal resistance network from heat transfer course on the topic of conduction to come up with equivalent homogenized orthotropic thermal conductivity values. Then it is important in the mesh to be sure the element coordinate system aligns properly to represent the x,y,z or 1,2,3 directions of the composite. In Mechanical, you can right mouse button on the geometry object and insert element orientation. Unless you were using Ansys Composite prep-post (which seems you are) which would allow you to setup layup and orientations, etc. Thank you.



  • sharveysharvey San Diego, CAMember
    edited September 18


    I wanted to point out that depending on the license you are using, you can use Ansys Material Designer to do homogenization both structural and thermal. Material Designer can be found in the Workbench Toolbox. The material could then be used in Ansys ACP.

    Thank you


  • Ahcene_94Ahcene_94 Member
    edited September 19

    Hello sharvey,

    Thank you so much for your response. Material Designer is really interesting as a modeling tool.

    I m lost because I don't understand why in my results obtained for the analysis of a composite pipe, the strains along the radius (Y and Z axis) are different while in the Engineering data, the limits of tensile strain along y and z axis are the same. (the pressure is applied over the entire circumference. )

    I tried the same problem in cylindrical coordinates but I got the same result.

    Do you have any explanation for my problem ?

  • I also think that it's necessary to have the same strain according to x and y axis because we have the same stress depending on the radius

  • sharveysharvey San Diego, CAMember


    The Strain limits will be used in failure criteria, so when you report the failure criteria you can see if failure is predicted, but for the solver to actually change the stiffness of the material (when the limit is reached) we need a failure model like the progressive damage or continuum damage mechanics material models. So the failure criteria is just a calculation, and does not affect the stiffness on it's own.

    Regarding seeing difference, have you checked the element orientation? You can insert a results quantity to request element orientation and you should be sure the triads are aligned as expected. Sorry if I repeat what I mentioned above, I just need not see confirmation if this was checked. One thing you can do is put in isotropic conductivity and thermal expansion, and verify you get the expected matching strains to each other. With uniform thermal condition, all temps equal) then you should should see the thermal strain to be alpha*dT. Put in a result on thermal strain to confirm this. You mechanical strains will be based on how the tube is constrained. Then proceed to the orthotropic values of conductivity and CTE. It things look peculiar you should check your element orientation. See if these suggestions. Help. Thank you.


  • Hello,

    I don't think I have a problem with the orientation of the axis system. You can see this on my screenshot.

  • sharveysharvey San Diego, CAMember

    Hello, if you insert a results under solution of coordinate system, element triad, you will get a plot. Notice how my element triads are aligned with global, and not cylindrical coordinate system. So, you will want to be sure this is correct to get proper thermal and structural behavior. This assumed solid mesh which appears is your case. For shell mesh, the z will be normal, but still the x and y may not align as you wish.

    How to fix this? Right click on geometry then pick element orientation. There you can can use the defined by to use a coordinate system or surface and edge guide.

    Please try and see if that helps. Thank you


  • Hi,

    Okay, thank you for all these explanations!

    Also, I would like to know if is this the right orientation of the coordinate system. Because my structure is a pipe that will be made by the filament winding process and the orientation of the fibers will be at 90° to the cylinder. 

    I'm wondering if my coordinate system should be aligned with the global system as shown in the picture above because the limits of stresses given in the Engineering Data will depend on the direction of our coordinate system, this is the most important I think to get the good results.

  • sharveysharvey San Diego, CAMember


    Ah good question. Sorry for confusion. I realize now that if you are using ACP, then in that tool you will be setting the fiber orientation. So once the layup comes from ACP to mechanical, the fiber/matrix orientation will be set (provided it is properly defined in ACP) The coordinate system of the element would be if you were not using ACP. Does that help clarify.



  • It's okay, Thank you !

Sign In or Register to comment.