Exporting CAD files from Solidworks for analysis in Mecway

traemand

Hi,

I'm currently trying out Mecway to figure out if it suits the kind of work i do.
I often need to analyze large assemblies of heavy duty vehicles, which i break down to smaller assemblies when possible.
Examples would be: vehicle chassis (welded steel square tubes) stresses, vehicle axle stresses, vehicle hitch stresses, etc.
With the current limitation of 1000 nodes, i mess around with simpler assemblies, say, 3 square tubes welded together.

I've gone through the tutorials, and read halfway through the manual - but i still have issues with succesfully analysing the imported CAD geometries. I use SolidWorks to model. I've tried exporting the parts of the assembly individually, but they all get imported to the part origin, and since i dont seem to be able to manually move the individual parts, i cant seem to place them correctly. I dont seem to be able to export the individual parts from the SolidWorks assembly while maintaining the relation to the assembly origin, so that all components would be imported in the correct place.

I've had luck with saving an assembly as a part (.sldpart), then saving that file as .step, then importing into Mecway. That way its 1 geometry, but if i then apply bonded contacts between the tubes, the analysis seems to run well.
Currently i'm limited with not knowing how to hide parts of the 1 geometry to select surfaces that are hidden, for bonding.
I'm thinking there must be a better workflow.

Can someone point me in the right direction?

traemand

I just realised that i was making it more difficult for myself by first saving the assembly as a part, and then exporting to .step. Simply saving the assembly as .step yields the same import in Mecway. I still struggle with manipulating the model once inside Mecway, so that i actually select surfaces that are not visible due to parts overlapping.

However, i still struggle with the importing of individual .step files from an assembly, and have them placed correctly relative to each other

Sergio

Hi @traemand, welcome to the forum. About exporting assemblies to Mecway, what I do normaly

1) If they are few parts, in the CAD I hide all and leave only one part of the assembly, and then export as stp with the option to only export visible parts, so the same for all the components. Then you can import each one in Mecway (all individual steps in only one import), and so you will be able to hide/show individuals parts in Mecway to make associative faces groups.
2) In cases with lot of parts, I import the assembly step in Salome (an open source preprocessor), where I can explode the assembly in his components, and make the meshes there. Salome is usefull to create meshes with coincident nodes for differents parts, so if they are welded parts, you could consider as a continuos part for a first analysis, and no need to set up a TIE or other bc in Mecway. So I mesh in Salome, and export the mesh to Mecway in UNV format. Salome has several tools to create structured meshes, shells, beams elements...that complement Mecway a lot.
3) There is a documented procedure in the forum to make the same with Gmsh (another open source preprocessor) for meshing assemblies with coincident nodes.
4) If you have an assembly with components joined by bolts/nuts, you could use the procedure 1 for the components, but all the bolts/nuts (that must be very simplified and bolt-nut a same part) in one step (so you will be able to hide/show every parts, and all bolts/nuts at the same time.


Regards

traemand

Hi Sergio,

Thanks again for your awesome feedback Sergio. I appreciate our contact over reddit.

1) Great advice! It worked flawlessly, although it is a cumbersome proces. I wonder if i can get a SolidWorks macro set up that suppresses all parts except 1 at a time, and saves the file as a .step, and then steps through all the components that way. That would be awesome.
2) I see - i have to look into Salome. I wish i was able to do all of it from inside Mecway. Would be neat to have the option to "Explode geometry into sub-geometries", or something.
3) Would that mean to mesh from inside Mecway but using the Gmsh option to somehow split the geometry up into separate meshes, or would i have to preprocess in Gmsh from outside of Mecway?
4) So essentially: Export one big .step file with all components hidden EXCEPT for the bolts and nuts, and then add contact for each bolt/nut connection to adjacents surfaces in Mecway?

One thing that really bugs me at the moment is the fact that the imported geometries are not highlighted individually when you click them in the tree. Only when i have a mesh can i see which is which. The parts i work with are not named "plate" or "cylinder" but rather "7407-5542" or the like. Any simple solution i haven't figured out yet?

traemand

Also, as i end up having quite a few bonded contacts: is there any way to have Mecway highligt which contacts are in question when you activate the bonded contact from the tree? It works as expected when activating either the slave or master.

Sergio

2) You have such "explode geometry into subgeometries" in Salome. You can even prepare shell models there, leaving one side of sheet metal parts, and then export as step to mesh and work in Mecway.
3) Now I don't remember, but look for the specific post, that was all explained there.
4) For bolted parts, there are several ways to do it. If you want to work with solid bolts, you must create a very simplified bolt, but with the nut in the same SW part (so you discard the TIE between nut/bolt), you should model also the washer diameter in that part, so in fact the hexa head/nut can become a cilindrical shape with washer diameter (less element count), So now, in SW you can export first the two parts separately, and then only one step for all the bolts, so in Mecway the bots will be a multibody part, but easier to mangane than several individual parts.
You can model also your bolts with a beams element and a spider of rigid beams, or one beam for the shank, and another beam element with biger diameter for head/nut. There is a specific post for the creations of spiders, and for bolt modeling using only beam elements.

For "seeing" the bonded contact, what I found easier is change the visualization to wireframe only (you could even change the model edge color to magenta for even easier visualization), and then select the TIE in the three, and should be hilighted in the model view.

Sergio

I have checked, and for getting a coincident mesh with separated/selectionable parts, must be done outside Mecway with Gmsh or Salome. You could do inside Mecway, but all the elements will be assigned to one component without easy way to separate or select it. My advice is to use Salome, as it easier and even in the last versions you can use also Gmsh within Salome.

LorenzoS

Hi traemand end Sergio

@Sergio I tried to explode "geometry into sub-geometries", and later I tried to mesh without results; where do i get lost?

I attached a rar of file .step .hdf and a picture.

Thanks

Lorenzo

Sergio

Hi, during the day will try to prepare a tutorial for meshing the assembly with coincident nodes in Salome and export to Mecway.

traemand

Great stuff Sergio!

A small update:
I figured out how to export large assemblies as individual .step files with the relative positions from the assembly file.
1) Save assembly as .sldpart
2) Use feature "Save bodies" and use the Auto-assign names (beware: subassemblies will by default SW naming convention need manual updating. Otherwise they will be named "bodies1" etc.)
3) Use the SolidWorks Task Scheduler, click Export files, add all the saved bodies, and choose step format
4) Import into Mecway!

As a test, to push the software, i imported a 247 part assembly of a large chassis into Mecway and sucessfully generated a default automesh. Impressive!

Sergio

The model look interesting, but workng with such cuantity of components will be a nighmare in Mecway. Remove all non structural components, and surely you will have to make the meshes very carefully (by hand each one) to have something usfull. The automesh will create too much elements and deformed due to the small radius of the profiles.

traemand

Yes, it is not for actual use. But it's nice to see that the software is capable of handling models of that size.

In what specific ways do you think that it will be a nightmare?

Sergio

And use simmetry, at least for building the meshes.

Sergio

Moving in the model tree, using the scrool bar for locating components or bc will make you very annoyed. For that kind of models the possibility of grouping components (the same as today for boundary conditions) would help a lot. And for assigning material to 234 components... :-( Probably will be easy to create a group with all the elements and assing only one basic steel to all by means of a CCX custom card.

Sergio

@Lorenzo, attached a tutorial for creating conformal meshes in Salome and exporting to Mecway

https://we.tl/t-v0FNRrOzLt

LorenzoS

@Sergio, great guide with pictures and description!
Thank you for taking the time to wrtite it
Now the export from Salome mecway is clearer
just a doubt, in the last slide how do you select all elements to "add elements to new component"?

Lorenzo

MMK66

Hi

The procedure I use in the case of Solid Edge, I export the step file to salome, in salome I give a hex 8 / hex grid to 20 parts, then I transfer it to gmesh and save to unv there and then Mecway reads these assemblies beautifully for each party, the mesh is clean. Later, I can narrow down selected areas in Mecway. For example, I divide into a 2cm grid, and I divide selected ones into one with 1mm tools in Mecway. I have not used it for a while, but the procedure I used is described on the forum. Without the use of salome, it will not be possible. Gmsh is a very good exporter, referred to as meshes, it serves as a catalyst, in which you can see whether the model has individual parts or is a monolith

traemand

@Sergio i see now what you mean. One thing that is maddening is that i can't seem to find a way to set "Meshing parameters", Material etc. with 1 click. Is it not possible to select multiple similar tree items at a time, and set the options for all of them at the same time? If not, then yes, that WILL be a nightmare... :-(

Sergio

@Lorenzo, in Mecway, first select the group in the model tree, the elements become selected in the model view. Now press the secondary button of the mouse over the selected elements in the model view, to bring up the contextual menu with the option to create a new component.
Another way would be select the group first, and then in the model tree, if you select the Components & Materials branch, an option to create a new component appears.

Sergio

@traemand, it´s not possible to do multiple selection in the model tree. What you could do is adjust the default options of mesh in the Tools/Option/Defaults windows to a more suitable values for most of your parts, and then only edit those that were not accurate meshed with the default ones. But again, that parts of the such must be meshed individually in Salome (at least those that are long profiles) in order to control the element quantity and distribution.

Sergio

@traemand, it´s not possible to do multiple selection in the model tree. What you could do is adjust the default options of mesh in the Tools/Option/Defaults windows to a more suitable values for most of your parts, and then only edit those that were not accurate meshed with the default ones. But again, that parts of the such must be meshed individually in Salome (at least those that are long profiles) in order to control the element quantity and distribution.

LorenzoS

@Sergio, ok i succeeded.
There is an area that needs to increase the detail of the mesh (as shown in the picture)
Do I need to return to Salome or can I change the mesh in Mecway?

Sergio

You could drag the nodes of some failed elements to make it acceptables directly in Mecway (or even delete the elements), but is easier to remesh in Salome with different parameters.

traemand

Beautiful tutorial @Sergio. I really appreciate the work you've put into it. Thank you!

Are you going to be making more like this? I think there's potential for YouTube channel :-)

Sergio

Forget about videos :-)

I was thinking in reformat and make a series of articles on my site/blog.

dculp

Sergio --

For "seeing" the bonded contact, what I found easier is change the visualization to wireframe only (you could even change the model edge color to magenta for even easier visualization), and then select the TIE in the three, and should be hilighted in the model view.

(August 10)

Do you mean that the TIE bonded surfaces will be highlighted or that the individual TIE bonded nodes will be highlighted?

Sergio

In the versions were the TIE was highlighted with small black balls, was easier to see if the element surfaces were hiden, and the mesh color was adjusted to cyan (same color as undeformed mesh by default). With this configuration I found easier to identify not only the TIE but also the surfaces related painted in blue.

JohnM

If you name your CONTACT or TIE surfaces using "sequential" names, for example, S101,S102,S103,S104... such that the surface pairs are S101/S102, then S103/104....
The surfaces will be listed in the Named Selection in surface pair order. You can then display your model as @dculp describes, and use the down air on your Named Selections to verify the pairs. This makes quick work out of verifying even hundreds of pairs.

dculp

Sergio --

I now understand the process to see the the small black balls for the TIE bonded nodes --
1. Click on a TIE bonded contact surface in the tree.
2. \Edit\Select nodes

This shows all of the nodes on the selected surface but not necessarily those that are actually tied. From my understanding, these can only be determined by analyzing the model and then looking for any slave nodes in WarnNodeMissTiedContact.nam. However, if the slave surface extends beyond the master surface then those "uncovered" slave nodes will be listed in WarnNodeMissTiedContact.nam, even if all of the nodes at the master-slave contact interfaces are correctly tied. (Of course, the model could be adjusted so that the slave surface doesn't extend beyond the master surface but this requires additional modeling effort. Still looking for a better method of detecting unbonded nodes ... )

dculp

Sergio --

From your post of August 11 (tutorial for creating conformal meshes in Salome and exporting to Mecway) -- https://we.tl/t-v0FNRrOzLt

I tried to access this but the site said "Transfer expired." Can you post this again (possibly as a more permanent file)?

Thanks,
Don C.

Sergio

https://we.tl/t-LIeS8U1LIz

Will try to upload to my site in the future.