3D Design

3D Design

ACP Pre peg Modeling

    • Sushil Sharma
      Subscriber

      I want to analyze Composite Wind turbine blades in fatigue.

      1. When I try to create a modeling group in workbench, I gott an error message( as shown in the screenshot). What this error mean,s, and how can i solve this problem.
      2. I want to vary the section thickness in longitudinal direction of my model. How can I do this?
    • bhagwantP
      Ansys Employee

      Hello Sushil ,

      Have you used shared topology in modelling?

      Looks like error is prompting that there are more than one bodies where topology didn't happened.

      Thanks

    • Reno Genest
      Ansys Employee

      Hello Sushil,

      You can vary the thickness by applying prepreg layers as you would do when building the composite layup in real life. One way is to create diifferent element sets for the regions where prepreg layers will be applied. Next, you create many Oriented Element Sets using the different Element Sets. Finally, you can add layers in different regions by selecting the appropriate Oriented Element Sets in Modeling Groups. 

      Another option is to use selection rules instead of Element Sets. 

      This is explained in the Ansys Composite PrePost course on the Ansys Learning Hub:

      https://jam8.sapjam.com/groups/YHNivy2FbzTCwBmZhqlMGS/overview_page/X59hQ2TTw5kCamrfUyAeA6

       

      If you don't have access to the Ansys Learning Hub, you will find videos on how to build a formula SAE composite chassis with ACP here:

      https://courses.ansys.com/index.php/courses/formula-sae-composite-monocoque-chassis-analysis/

       

      Let me know how it goes.

       

      Reno.

    • Sushil Sharma
      Subscriber

      Thank you

      While using the selection rule how to consider the abrupt section change. I want to create sandwich panel "section rule" will create notch in each dividing plane. Does it effect on fatigue analysis of the blade?

    • Reno Genest
      Ansys Employee

       

      Hello Sushil,

      You can create abrupt section changes by defining a different number of layers for each oriented element sets. This will lead to ply drop off. Here are 2 ways of doing it:

      Splitting the surface in SpaceClaim:

      I think the best way of doing it is to slice your surface geometry in SpaceClaim to have all the regions of the surface where you have different layups (different number of plies). You want to split the face without creating new surface bodies:

       

      Then, you create named selections in Mechanical for each region. The named selections will transfer to ACP as element sets. You can then use the different element sets to create the Oriented element sets needed to build the layup. This is the best way because if you refine the mesh in Mechanical, the element sets will update properly based on the named selections in Mechanical. Let me know if you have questions about this process.

      Using selection rules:

      Using selection rules is the second best option I think. It will keep the regions almost the same when refining the mesh, but you may have some elements that are not picked up by the selection rule and you end up with a jagged region. This may be okay for early design iterations when you don’t know exactly where the boundary of each region will be. So, selection rules is more flexible and allow you to quickly change the boundary of each region.

      So, with selection rules you don’t need to split the surface in SpaceClaim and you don’t need to have named selections in Mechanical. I created an example of a square plate with 3 regions (left, middle, and right). Here is the left region selection rule:

       

      Once you created the selection rules, you can create the oriented selection sets:

      On the General tab, you select all elements as element set and define the other inputs (point, direction, rosette) as usual. Then, you move to the Rules tab and select the appropriate selection rule for the oriented selection set:

       

      You do the same process for all regions and then you can build the layup (add plies in Modeling Groups):

      Then, when you create the solid model, you have drop off options. The default are:

      Which leads to the following:

      The ply drop offs will happen over the length of your element. So, if you have large elements, the drop off will be smoother and if you have small elements the drop off will be more abrupt.

      You can also disable the drop off to get an abrupt drop:

       

      But, this is not a good design; it will lead to stress concentration which is not good for fatigue life. You should have a nice and smooth transition in your composite layup.

      I recommend you create a simple plate model like the one above and “play” with the different options and see what works best for you. There are many ways to do things in ACP.

       

      Let me know how it goes.

       

      Reno.

       

    • Sushil Sharma
      Subscriber

      Thank you, Reno.

      I have another question regarding the modeling of the sandwich panel (Foam in between the UD carbon fiber layer). I tried to model it using selection rule. When I try to vary the element thickness by adding the extra layer on the root section, ANSYS adds that section to the previously modeled throughout section. At the root part, my section shows (carbon fiber layer+core+carbon fiber layer+ carbon fiber layer+core+carbon fiber layer). That is, my model has two independent sandwich elements on the root. How can I correct this to my element so that the core will be added to the core part and outer skin to the outer skin part so my model has one (carbon fiber layer+core+carbon fiber layer) with variable thickness?

       

    • Reno Genest
      Ansys Employee

      Hello Sushil,

      I am not sure I fully understand the problem. You have 2 sandwiches instead of one? Could you send an image? 

      How is this part built in real life? How are the layers applied? How is the foam positioned? If you follow the manufacturing procedure in ACP, you should get good results.

      The oriented element sets will determine where the foam is located.

      Let me know how it goes.

      Reno.

    • Reno Genest
      Ansys Employee

      Hello Sushil,

      Are you trying to build something like the following?

       

      In the above model, the foam is applied to all elements (oriented set "All"):

       

      Let me know if this helps or not.

       

      Reno.

    • Reno Genest
      Ansys Employee

       

      Hello Sushil,

      If the composite layers are positioned on top and bottom surfaces of the foam core, you can start by adding the foam core as the first “layer” on the surface. You can apply half the foam core thickness in the “up” direction and half the core thickness in the “down” direction from the surface. Then, you can add the carbon layers on top and bottom surfaces. The result is as follows:

       

      You will need to create double the amount of Oriented selection sets; some for the “up” direction, and others for the “down” direction:

       

      Let me know if this helps or not.

       

      Reno.

       

    • Sushil Sharma
      Subscriber

      I want to model similar to this but also want to vary the foam's thickness.

    • Reno Genest
      Ansys Employee

      Hello Sushil,

      It is basically the same process for variable thickness foam:

      Is it what you are looking for?

       

      Reno.

    • Reno Genest
      Ansys Employee

      Hello Sushil,

      If your core geometry is complex, you could create the 3D geometry of the foam core in SpaceClaim and then create surfaces on top and bottom faces of the foam core:

       

      You can select "Share" for the share topology setting to have conformal mesh between the solid core and the surfaces. Without "Share", you need to define bonded contacts between the foam core and the surfaces (used to define the carbon  layup).

      Then, in Mechanical, you can mesh the model and create named selections:

      In ACP, you will only see the top and bottom surfaces used to create the composite layup:

       

      But, when you link ACP pre to a Static Structural system, the foam core will show up in Mechanical:

       

      Let me know how it goes.

       

      Reno.

    • Reno Genest
      Ansys Employee

      Hello Sushil,

      Yet another way to do it is to build the composite layup and foam core on a surface like we were doing. Then create a 3D model of the finished composite sandwich, mesh it, and import the 3D solid mesh in ACP to map the composite layup onto the solid mesh. You will find more information about this technique in the help:

      https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v231/en/acp_ug/acp_ex_mapped_composite_solid.html

       

      Let me know how it goes.

       

      Reno.

    • Sushil Sharma
      Subscriber

      Thank you for getting back to me. I will write again about where I will be stuck.

Viewing 13 reply threads
  • You must be logged in to reply to this topic.