Meshing with shell elements

Andrea

Hi!
I meshed on Mw a basket with shell elements. The problem is that the elements aren't connected.
Meshing into Salome, creating a fuse function of the all shells, the mesh is correct and continuous.
So I ask if anyone had the same problem and what's is necessary to do by CAD to avoid mesh discontinuity.

I had the same problems same time ago but I never solved it into Mecway

Andrea

Here the final mesh...good results in 2 minutes

Sergio

Have the same concerns on Mecway, the clasic solutions is use Salome or Roshaz if you want 100% quads. Have tried lot of configurations while exporting from the CAD but none works.

Regards

Andrea

Hi Sergio!
The problem is not to obtain all quads. The problem is the mesh which is disconnected between one face to another at the common edge/s. Surely depends from step model because operating a boolean operation in Salome (fuse) the resultant mesh is continuous.
Those basket will be enterely welded and I need continuous mesh and I need to avoid bonded contacts.

VMH

Andrea, this probably not an answer but just an option:  I use FreeCAD and "union" surface parts together and then import the exported .step file to Mecway.

VMH

This is a video for union the surface model in FreeCAD:

Andrea

Yes.
This was the problem which depends from CAD model.

Now I have to apply different thickness to some faces but, if I remember what wrote Victor, it is possible creating a New Component. These faces must be a part of a group of elements.

Regards, Andrea

nwedding

Hi all. I often need to analyze weldments made of plates or structural shapes. I'd like to take the 3d file and get a 2d mesh at the midplane of the plates. Algor used to have a feature that would do this automatically, but it didn't always work so well. Andrea's model posted here looks like he's doing the same kind of thing. Can someone give me some instruction on how to make this happen in Mecway, Salome, Gmesh, or any other software that might be available? It would be great to have the meshes match at the edges so the parts are joined. Otherwise, I can put a bonded contact at the edges. Either way, I need to get the stresses and deformations in the plates and the edge forces for weld sizing. I have tried to figure this out for some time and have not had any luck. I also have no experience with the 3rd party meshers, so I may just not know what I'm doing with them. Please help if you can. The attached is an example of a weldment I'm trying to analyze. 

Sergio

If you want to work with shell elements, then is better to do the CAD model directly using surfaces and not as a solid. In that cases I prefer to work with one side of the model (and not midplane), and tell the preprocessador the thickness direction. Using that approach the dimension of the model will be directly the "specificated or drawing dimension" less prone to mistakes as in he case of midplane. Also for changing the thickness, the dimension will still be ok, and for contact also is easier to setup and avoid mistakes due to the thickness.


Mecway doesn't allow to indicate the thickness direction, it assume is the midplane, but can be changed by means of CCX custom edits.

nwedding

That's what I was afraid of. I was hoping that one of the meshing engines could do it for me from my solid. Thanks Sergio!

Sergio

High end mesher as NX or even SolidWorks allow you to create midplane from solid parts (but is not perfect at all). But even for CAD modeling I use the same approach, first model as surface one side of the part (normally the one that will be in contact with other parts in the assembly, so that side is "fixed"), then at the end use some cad operation to convert the surface to a solid part with constant thiknnes. Then I can use that surface for FEA, and if I need to change the thickness then will not affect the matching part on the assembly.

Victor

Although you can't specify thickness always being from one face in Mecway, you can use Shell offset in Element properties to move the midplane to one of the surfaces. It works for both the internal solver and CCX. So you can make a surface mesh of just the outside or inside then move the midplane to its correct location. It does introduce some error at corners where the offset elements end up intersecting or separated from each other so their dimensions are altered.

nwedding

Thanks! I'll give those methods a try.

JRP

Is there anything new on importing surfaces to Mecway as STEP model?

I'm still having problems with not being able to join all the surfaces together in Solidworks into one surface. I then save it as STEP model and when I import it to Mecway and mesh it, I get dislocated nodes on surface edges, that were not before joined. The reason Solidworks doesn't allow to join surfaces is because there can't be more than two surfaces joined on one edge. There is no problem where one surface has more faces, which are created with split line command. I usually use this for some preparations for easier selection in Mecway.

I use a procedure in which I make midplane surfaces for sheet metal plates. I prepare all of the surfaces I know I will need for load and constraint application and then I save it as STEP file.

Maybe I should model this from beginning in Mecway, since it is relatively simple structure. But sometimes I have more complex models and preparation of surfaces in CAD is good, because meshing is not simple in Mecway.

Does anybody have any recommendations for easier model generation?

Andrea

For what I know creating surfaces in CAD environment you haven't intersection edges. So importing directly on Mecway the faces are treated as separated surface bodies and the mesh is incongruent.
As you wrote is necessary to split the surfaces but sometimes is a hard work.
I never find a faster solution than to import step file into Salome and apply "fuse" command.

Victor

If you use Gmsh, it makes compatible meshes on adjacent edges where they have the same length. In this example, there are some patches that break up the lines so it doesn't always match, but you can see the meshes are aligned in the other places. So you can split surfaces in CAD to get them all matching then merge nodes after meshing.

JRP

Thanks for answers.

Let me explain in some more detail how I break all the surfaces already in CAD (Solidworks). There are two possibilities:
1) You make separate surfaces with intersecting (NOT SAME) edges. If you can join these edges together, then there is no problem in Mecway. If edges cannot be joined, then Mecway meshes edges with nodes very close together usually. You have to zoom in to see or use the command for viewing open crakcs. This is sometimes solvable with combining nodes with 0,5 mm tolerance and then again check of all edges with open crack command.
2) In CAD one surface can be split to many faces. In Solidworks that is split line command. That means that the edges of different faces are the same because they belong to the same surface. But problem is that if you split one surface, you usually have to split all other that are adjacent or you get problems with nodes further apart and not being able to combine them.

Victor and Andrea, can you please explain both procedures in some steps. I never used Gmsh or Salome before and any help would be useful. Thanks in advance.

Andrea

A short video that explains the procedure



PS The second is better defined by "partially splitted"

JRP

Thanks Andrea very much for your time and effort. I will try this and report back soon.

VMH

JRP,

You can import your step file into FreeCAD. Then go to the part workbench, select the items, and click on the Union button. It will connect your surfaces. There will be a warning message about connecting non solid but that's okay. I have used this very often.

JRP

Hello VMH,

I've tried your solution, but it seems I get it wrong somewhere, because I get the same result.

I import my STEP model to FreeCAD and then select whole geometry. I press union command and I get error shown on screenshot. After that I get empty workspace with no geometry and failed fusion command on the left. I decided to export STEP anyway and it worked, but when I import it to Mecway, I still get same problem on same edges as before. Nontheway, at first I thought it worked, because STEP looks as if it has all edges combined, because they are different color when I open it in Solidworks (black and not light blue as before).

Andrea

Takes into account another aspect: often is necessary to assign different properties and/or thickness to the faces. You can do it into Mecway but creating groups on Salome and meshing within Salome, you will find groups of nodes or elements inside "named selection" folder in Mecway.
Meshing in Salome is not simple but is more powerful and is possible to obtain full quads or full hexa....I repeat it's an hard job

VMH

JRP,

See attachment and YouTube link below. I use FreeCAD version 0.16. They did alot of changes in FreeCAD version 0.17 that I didn't look into them yet so I still use version 0.16. Note that when exporting the step file from FreeCAD, I used the same name so Mecway updated the step file automatically (sometime I have to click reload). I also changed my unit to millimeters to match your Mecway settings (I uses inches). Also note that I first meshed with quadratic just to see if it mesh okay and it did besides the midside nodes of the triangle shapes didnt connect to adjacents. I then remeshed with your original (without quadratic) and it meshed okay too. I use quadratic whenever I can by default because it gives better reaults. Hope this help.

Victor,

For some reasons when I use quadratic surface meshing, the triangle shapes are not attached (see YouTube link below). I usually have to merge the node for them to connect as seen in the YouTube link below).

VMH

Files attached. Had to zipped the FreeCAD file since Mecway doesn't allow that file extension to be uploaded.

JRP

That's great VMH. It works. Thank you for your time with making the video. Which software do you guys use for screen video filming?

I had to change one setting in FreeCAD, because it did a compound merge at import of original STEP file and I had only one component, not multiple surfaces as was shown in your video. Check screenshot for more info. Basic point is, that it also works in FreeCAD 0.18. After import in Mecway I get good mesh with no misfitted nodes. I've checked with open crakcs and trying to merge nodes and the number stayed the same for quite big tolerance.
I would like to say that I try to knit together as much surfaces as possible in Solidworks CAD, so I get as few of them as possible. But it looks like FreeCAD writes somehow in STEP file after using union command, that common surface edges are the same and Mecway recognizes it in meshing procedure. If I import this corrected STEP back to Solidworks, it is still made out of same number of surfaces as it was before editing in FreeCAD.

I have one more question for one setting I've seen in your video (check other screenshot). You set min. nr. of el. per edge and per curve to 0.001. I've didn't get a simple answer to this day, what is a purpouse of this setting. Maybe Victor or some of you guys can explain from experiences, how does this setting reflect on mesh quality.

Thanks for all the help. This is great news for me now. I will make my FEM models easier and better with that union function in FreeCAD. Maybe somebody else will find this topic useful.

VMH

JRP,

There's usually 3 steps I used before uploading to YouTube. All softwares referenced below are free.

1) Screen record at the highest available settings using ActivePresenter. End and save the recording without exporting (exporting take some time to encode and process but the end quality is just okay and still have large file size so I skipped it). There should be a MKV and audio files in the local Document folder under ActivePresenter under your selected name for your screen recording session after you save.

2) I use MKVToolNix to combine (kit) the video and audio together.

3) I use HandBrake to compress output file from the MKV kit to MP4 to upload to YouTube. Depending on your setting, the video quality loss is minimal and file size is much smaller so the YouTube upload time is much shorter.

If there is no audio needed for the YouTube video, then I skip Step 2 and go from Step 1 to Step 3 using the MKV file without the audio.

As for the minimum number of elements per curve and per edge, it's all depend on your preferences of the final mesh. The higher the values, the more elements per curve or per edge which result in higher elements at areas we may not need and result in larger model and longer solving time. The lower value usually yield more uniform mesh depending on the actual geometry.

I'll send a comparison later.

VMH

JRP,

See YouTube below for Minimum Number of Element per Curve and per Edge.

JRP

Nice video VMH. I'm sure it will be useful for other user. A proposal maybe for Victor to create some sort of database of these videos and other things that are not all written in manual. It is hard to search for them on the forum when you don't know exactly what you are looking for.

And thanks for video editing info. I will take a look.

Victor

Google search is probably better than the forum's. This thread is near the top of the page for "mecway shell mesh edges video".

I'm also collecting some of them on the Mecway YouTube channel https://youtube.com/channel/UC8tXqfFUUYNb1kv5X4GLi3w

JRP

Yes, I usually use google for all my forum searches. You just need to use specific site search, like:

"mecway shell mesh site:http://mecway.com/forum"

mike262

I was having a few problems with my shell mesh. I read this thread and thought i would have a go at using Salome and it worked pretty well!.

I started off with a surface model in onshape made up of lots of separate parts.

I tried loading them in to mecway individually and meshing them with bonded contacts but this proved quite tedious and difficult. I tried Salome without having previously used it...i loaded in the individual surfaces and fused them into a single step file.

I had to break this up into lots of different named selections and components but it wasnt too difficult and i was able to achieve a good mesh that gave results in accordance with previous analysis i had done.