how to combine two types of elements in meshing 1

[alinalin]

Can I mesh an area with shell elements and its edge with beam elements? I use ANSYS to mesh one edge of the area first using 1D beam element, and then mesh the area using 2D shell element. In this way, the nodes generated from the beams elements, and the nodes generated from shell elements both exist in meshing. Although the edge is on the area, the nodes of beam elements are not attached to the area when I apply loads to area and solve. If I mesh the area first and the edge later, the result is the same. Is there any way that I can specify some nodes on an area and mesh the area, which includes these nodes? The area contains thousands’ nodes and I want to specify some nodes at some locations.

Thank you for any input!

 

[cbrn]

Hi,
first of all, check that you don't have overlapping lines in your geometry. Before meshing, due to the fact that you don't want separate boundary lines from the surface, merge the entities (keypoints and lines specifically).
At this point, there is no reason why Ansys should build non-corresponding meshes, but in order to be 100% sure, impose a fixed number of elements on the edges.
Warning: check in the Help how the DOF coupling between line-elems and 2D-elems works.

Regards

 

[alinalin]

Thank you for the reply.

You are right. I can use DOF coupling for the nodes of beam elements and shell elements at the edges. This requires the nodes of beam elements and nodes of shell elements are at the same location.

 

[cbrn]

Hi,
yes, this is one possible way.
If the element nodes' DOFs match (see the Help for each of the two types of elems you are using), then you can also MERGE the coincident nodes. It would be easier, faster and computationally much more efficient. But the elements' DOFs must match...

Regards

 

[Badri07]

HI Cbrn,

Further to your post,i would appreciate if you could let me know how to do i combine beam to solid elements.i am using ansyswb.

i am not sure how to proceed with that in workbench.

Thank you

Regards
Badri07.

 

[cbrn]

Hi,
Badri07, neither do I. For mixed-type elem analyses, I'm used to Classical. Sorry not to be of help...

Regards

 

[alinalin]

Hi, Cbrn.
Thank you for the reply.

The DOF of these two elements are the same. I can couple these DOF at nodes. But I meet another problem. I can not create nodes of shell elements at the location of nodes of beam elements. I first create nodes of beam elements. Then I create the nodes at the edge of curve surface. These nodes are not equally spaced and I can not generate them by using mesh control of line or area.

Alternatively, I tried to create hard points on the 3D surface. However, the curve surface can not be meshed even with only one hard point on the surface. If there any way that I can specify a location for a node and generate area meshing which pass the specified node? I tried hard point on 2D surface, it works. However, for 3D curve surface, it is not working.

 

[cbrn]

Hi,
Alinalin, I don't exactly understand the problems you are facing. Could you post the log file or post the location where to have a look at your db file? If you need I can post a simple example, but the fact is that right now I'm not so sure I've fully understood your point...

Regards

 

[alinalin]

Hi, Cbrn!

The following is the input file. I made this simple file for the purpose of understanding. My problem is to create meshing that contains nodes at specified location (certain coordinate, on a line of surface, etc.). I don't know how to realize this objective. Hard point might be one way of doing that. But after I generate a hard point on my 3D surface, the surface can not be meshed.

Please read the input file below.

Thank you very much!

/PREP7

ET,1,SHELL63
R,1,0.0042,0.0042,0.0042,0.0042
MP,EX,1,25E6
MP,PRXY,1,0.25

K,1,0.0,0.0,0.0
K,2,13.08,31.08,0.0
K,3,37.68,52.56,0.0
K,4,61.68,66.96,0.0
K,5,85.68,78.6,0.0
K,6,109.68,88.56,0.0
K,7,133.68,97.44,0.0
K,8,157.68,105.36,0.0
K,9,181.68,112.56,0.0
K,10,205.68,119.28,0.0
K,11,229.68,125.52,0.0
K,12,253.68,131.28,0.0
K,13,277.68,136.8,0.0
K,14,301.68,141.96,0.0
K,15,325.68,146.76,0.0
K,16,349.68,151.32,0.0
K,17,373.68,155.64,0.0
K,18,397.68,159.72,0.0
K,19,421.68,163.56,0.0
K,20,445.68,167.28,0.0
K,21,469.68,170.76,0.0

K,22,493.68,174.12,0.0
K,23,517.68,177.24,0.0
K,24,541.68,180.24,0.0
K,25,565.68,183.12,0.0
K,26,589.68,185.76,0.0
K,27,613.68,188.28,0.0
K,28,637.68,190.56,0.0

FLST,3,28,3

*do,i,1,28,1
FITEM,3,i
*enddo

BSPLIN, ,P51X

k,32,60,0,0

FLST,2,1,4,ORDE,1
FITEM,2,1
FLST,8,2,3
FITEM,8,1
FITEM,8,32
AROTAT,P51X, , , , , ,P51X, ,360, ,

! Create hard points

HPTCREATE,LINE,1,40,RATIO,0.5

!TYPE,1
!REAL,1
!MAT,1
!Esize,15,0,
!AMESH,1,4

FINISH

 

[cbrn]

Hi,
OK, I think it's clear now. I haven't run your logfile yet, but there is one command that is clearly wrong for what you want to do: you don't specify the number of divisions along the edges, only the global element "size".
The "ESIZE" command with the first argument filled won't, in fact, give elements of the same "edge length" because in the case of line-elems, ESIZE is of course exactly the elem length, whereas in 2D (and 3D) other considerations like element aspect ratio etc condition the final shape of each elem so that the edge length is not necessarily matching 100% the "ESIZE".
Instead, issue a ESIZE,,ndiv on each line you want to subdivide. Supposing that your surface has 4 edges, the NDIV on each pair of "opposite" edges need not to be the same: it has to be the same only if you want to quad-mesh the area.
If I have some time today, later on I'll post you the modified logfile.
I also suggest that you give another read to the Help section dealing with the meshing techniques. It's complicated but extremely complete.

Regards

 

[alinalin]

Hi, CBrn!
I appciate your help on this problem.

But my meshing can not be generated by using "ESIZE, NDIV". I have different element sizes on a line and I only want to create nodes at specified location. These nodes are not equally spaced. This can not be realized by "ESIZE, NDIV".

In another way, the problem can also be described as: I want to generate a 3D meshing which contains nodes at certatin locations. I need these nodes to apply loads. How do I generate a meshing which has specified nodes?

Thanks again!

 

[cbrn]

Hi,
thanx 4 clarification.
you could proceed like that:
- build nodes at coordinates using "direct generation" ("N" command), if you know their coordinates, OR:
- build keypoints at every location on surface edges where you want nodes to be put. I think it's better you do that in your CAD system, so you will have each surface edge "broken" in a multitude of small curved segments. Then mesh all lines by specifying ESIZE,,1 i.e. one single elem per line (also you can select only those segments where the extremity nodes are too distant and issue a ESIZE,,n to make a finer mesh there in between, knowing that this number of divisions doesn't annoy you because you already have the extremity nodes at their correct location).
- at this point you are ready to mesh the edges with line-elems.
- before meshing the surface, CONCATENATE the small segments belonging to the same edge. If you build concatenations so that the surface is enclosed by 4 "concatenated edges", then remember you can quad-mesh the surface (Mapped Mesh in Ansys terminology)
- if your CAD system supports this functionality, you could also subdivide the surface with u-v curves, then import it into ANSYS and direct-generate nodes and elements.

Hope this helps...

Regards

 

[alinalin]

Hi, Cbrn!

Thank you for the suggestion. It is very helpful.

Actually, I divided the lines to small segements, and I meshed the surface and its edge by specifying element size on lines. I tried to use hard point, but it didn't work for 3D curve surface.

I still have a few questions.
1. The warning of ANSYS said that "Real constant2 referenced by at least element types 2 and 1". My Element type 1 is shell element, Element type 2 is beam element. The real constants of these two types are of course different. (These two elements share one or more nodes). What does this mean in the warning message?

2. Another warning is "Coefficient ratio exceeds 1.0e8 - Check results." I checked my model there is no rigid body motion. What is the coefficient ratio? (PS, I used nonlinear element in model.)

3. What CAD software can "subdivide the surface with u-v curves"?

Thank you very much!

 

[cbrn]

Hi,
1- probably there was some small mistake when assigning elem type & real constant during line- or area-mesh. In fact, if you use GUI dialog boxes, things can get a little tricky because you can't really perceive what Ansys is assigning for the fields you don't explicitly set. For example, if you were to use a SOLID95 element, which doesn't require any real constant, and this elem type was created as, say, elem type number 1, then in the dialog box you would set "element type number -> 1" and leave all other fields unchanged, but then how would you know what Ansys assigns to the solid in the field "real constant number" (as you can see, by default it says "1"...). I really prefer setting things like that via Commands.
However, you can check the "correctness" of the mesh via the check commands.
2- In the global assembled matrix, the ratio between the max stiffness coefficient Kij(max) and the minimum one Kij(min) is greater than Ansys' check threshold. This indicates that there is a "weak" term in the system. But that doesn't necessarily means that there is a problem. With such high ratio, iterative solvers may have some difficulty to converge: if you don't have very big models, you can use sparse (direct) solver instead. Obey to Ansys, however: consider the results with "suspicion": if everything looks OK (i.e. is compatible with the physics laws !!!) then you can validate your solution.
3- From what I know, almost all "good" CADs can create u-v curves from a surface and then use them to subdivide the surface itself. I know for sure, at least: UG 16,17,18,NX,NX2,NX3,NX4,NX5..., Catia v.4 / v.5, Solidworks 2004,2005,2006..., Pro/E 20,21,2001,Wildfire1,Wildfire2...
A warning, however: the u-v extraction method may work for you only if the nodes at the opposite edges are identically spaced (well, it may also work in any general case, if the CAD is also able to create hard-points along a CURVE at defined u-coordinate values: in fact, what you really need is to subdivide the edges, not necessarily the surface itself.

Hope this helps,

Regards

 

[alinalin]

Cbrn, Thank you for the answer.

1. I used Command instead of GUI to assign the real constants to the two types of elements. So, there are two different sets of real constants for two types of elements which share the same nodes. These elements don't need to have the same real constants, right?

2. I am not sure how to create u-v curves from a surface using Solidworks. Is there any way that I can import line model of Solidworks (the Solidworks model only has 3D curves, and doesn't contain surface, doesn't contain solids) into ANSYS? I know that IGES, Para solid, and SAT files can be imported into ANSYS. But is it possible if there is no solid and no surface, and only curves?

Thank you for your help.

 

[cbrn]

Hi,
1- Things sound correct as you are doing them.
2- For sure, IGES transfer will work in importing line-model into Classical. Right now I don't remember if Parasolid can do this also, but I don't think so. However, the IGES choice in this case is optimal, unless you have SolidWorks curves with a spline-order higher than the one Ansys can handle.
Note that, if you are able to create the surface in Ansys from your Solidworks curves, then for sure you also are able to create the same surface in Solidworks itself (with much more "power and control"...). The geometrical kernel of Classical, in fact, is a dinosaur compared to nowadays modelers such as Solidworks.

Regards

 

[alinalin]

Hi, Cbrn,
Thank you again!

I tried it. You are right. I imported IGES file with only curves into ANSYS. I used to think that IGES only works for surfaces. The ANSYS geometry generation is not very powerful.