Stuck? 
support@mecway.com
support@mecway.com
Mecway
FEA
Composite questions
Hi all,
I'm trying to do some calculations on a (Carbon Fiber) composite part. I've read the two threads I could find about this topic at this thread (https://mecway.com/forum/discussion/comment/1685/#Comment_1685 and http://mecway.com/forum/discussion/comment/1609/#Comment_1609). I made a manual mesh based model myself (just a straight plate) and that seems to work well. However, I want to do some simulation at more complex (CAD based) models. I couldn't find much information about this, so maybe somebody can help me.
Basically my question is, how to mesh a UD 6 layer CF CAD-part in such a way the local x-axis are pointing in the direction of how the fibers will be orientated when you produce such a part.
Some subquestions:
1. What is the best element type to use? I think by experimenting it works best by selecting quad domiant under Mesh parameters, and also Quadratic elements and fit midside nodes. But maybe this isn't how it should be?
2. Because CF is anisotropic, the local orientation of the x and y axis of the meshed elements is important (correct?), which isn't the case for metals etc.
3. See atached picture/file, with minimum elements per curve and edge at 0 (and above mentioned settings) this gives the best orientation of the elements. However, some elements (in the fillet area for example) don't have the x orientation in the right direction (fiber direction). How to solve this? I know you can do some corrections by hand, but that would be very hard with complex 3D shapes. Is there a better way to do this?
4. I think I've found out in case of a CAD based mesh the material (lay-up) is placed at both the upper and botom side of the part. Which means if you describe the material with all 6 layers, Mecway places 6 at top and 6 at bottom, so the part wil be 12 layers thick. This doesn't happen with a hand-meshed part, where you kind of model the "plane" of where the layers are placed. Is this correct?
I hope my questions are making some sense.
I'm trying to do some calculations on a (Carbon Fiber) composite part. I've read the two threads I could find about this topic at this thread (https://mecway.com/forum/discussion/comment/1685/#Comment_1685 and http://mecway.com/forum/discussion/comment/1609/#Comment_1609). I made a manual mesh based model myself (just a straight plate) and that seems to work well. However, I want to do some simulation at more complex (CAD based) models. I couldn't find much information about this, so maybe somebody can help me.
Basically my question is, how to mesh a UD 6 layer CF CAD-part in such a way the local x-axis are pointing in the direction of how the fibers will be orientated when you produce such a part.
Some subquestions:
1. What is the best element type to use? I think by experimenting it works best by selecting quad domiant under Mesh parameters, and also Quadratic elements and fit midside nodes. But maybe this isn't how it should be?
2. Because CF is anisotropic, the local orientation of the x and y axis of the meshed elements is important (correct?), which isn't the case for metals etc.
3. See atached picture/file, with minimum elements per curve and edge at 0 (and above mentioned settings) this gives the best orientation of the elements. However, some elements (in the fillet area for example) don't have the x orientation in the right direction (fiber direction). How to solve this? I know you can do some corrections by hand, but that would be very hard with complex 3D shapes. Is there a better way to do this?
4. I think I've found out in case of a CAD based mesh the material (lay-up) is placed at both the upper and botom side of the part. Which means if you describe the material with all 6 layers, Mecway places 6 at top and 6 at bottom, so the part wil be 12 layers thick. This doesn't happen with a hand-meshed part, where you kind of model the "plane" of where the layers are placed. Is this correct?
I hope my questions are making some sense.
Howdy, Stranger!
It looks like you're new here. If you want to get involved, click one of these buttons!
Comments
1. Yes, I think quad8 (quadratic, quad dominant) is best. Quad4 may be OK too. Yes, turn on Fit midside nodes to geometry. That's only off because it sometimes makes badly shaped elements which won't solve.
2. Yes
3. The default element orientations are effectively arbitrary so don't use them. Instead, there are two ways to define the direction of the U (local x) axis:
a) Select elements, right click one, click Element properties, enter the direction vector there under Orientation.
b) Add an Element orientation under Loads & constraints. This way is newer and allows you to define it by a formula as a function of position, so you might have them uniform along the straight part but rotated around the circular part.
4. Your model may have solid walls. In that case, Mecway meshes the entire surface - inside, outside, and edges. You could either use a surface model instead, or delete all the faces you don't want after meshing, eg all the inside and edge ones. Edit -> Edge detecting selection, Edit -> Select elements, then Edit -> Invert selection can make this fairly easy.
However I don't see how I change the orientation in case of a complex 3D shape. For example I attached a motorcycle wheel (see file). Let's say this is a aluminum wheel and I want to change the rim for a CF rim. I made two parts; Hub and spokes are out of aluminum (orientation of elements not relevant), rim of UD CF. The spokes and hub are meshed with the Gmesh option. Rim is a surface mesh. Since you mentioned I shouldn't use the default element orientations, how to orientate these the right way? I've no idea of a formula that can fix this for me...
To open this dialog box ,put cursor on top of the elements , right button and element properties menu
So disla's (0,z,-y) formulas would make the U axis in the circumferential direction despite the crooked elements. But that's only available with the Loads & constraints -> New element orientation option, not through Element properties.
Since the mesher can't find the midplane, you could either move the CAD model, or use Shell offset in Element properties to get the solver to treat the shells as being offset.