Meshing Compsolid in Salome 3.2.2
- Fergus Rhodes
- Topic Author
- Offline
- New Member
-
Less
More
- Posts: 9
- Thank you received: 0
16 years 6 months ago #1386
by Fergus Rhodes
Meshing Compsolid in Salome 3.2.2 was created by Fergus Rhodes
Hi,
I've got a step assembly model I've imported into Salome as a Compsolid. I explode this into individuals solids, mesh and then create a volume group for each solid to assign material properties. However the mesh does not join between the solids, so it will not solve.
If I use the Fuse command in the geometry module to fuse these solids togeather I then get a mesh which is joined between all the solids. This will solve OK. The problem is I don't seem to be able to assign a group to each solid (presumably as they have been fused).
What is the correct way to mesh a Compsolid ? Is there another way, other than the Fuse command, to ensure that a single cohesive (joined up) mesh is formed?
I've got a step assembly model I've imported into Salome as a Compsolid. I explode this into individuals solids, mesh and then create a volume group for each solid to assign material properties. However the mesh does not join between the solids, so it will not solve.
If I use the Fuse command in the geometry module to fuse these solids togeather I then get a mesh which is joined between all the solids. This will solve OK. The problem is I don't seem to be able to assign a group to each solid (presumably as they have been fused).
What is the correct way to mesh a Compsolid ? Is there another way, other than the Fuse command, to ensure that a single cohesive (joined up) mesh is formed?
Please Log in or Create an account to join the conversation.
- Fergus Rhodes
- Topic Author
- Offline
- New Member
-
Less
More
- Posts: 9
- Thank you received: 0
16 years 6 months ago #1387
by Fergus Rhodes
Replied by Fergus Rhodes on topic Re:Meshing Compsolid in Salome 3.2.2
Hi,
Think I've figured this out. Work flow for importing a Step assembly and creating a unified mesh of distinct volumes (eg. for different material properties), seems to be 1) Import .stp into Salome 2) Explode to Solids and Faces 3) Fuse Solids (multiple fuse operations are required to fuse multiple solids) 4) Partition the Fuse, using the faces from (2) to divide the body into individual solids (Partition the Fuse, then partition the subsequent partition to divide into multiple solids) 5) Explode the final partition into Solids and Faces 6) Mesh the (final) Partition 7) Define volume groups in the mesh based on the individual solids in the partition 8) Select faces for the boundary conditions from the faces exploded inside the partition.
This solved OK. Does anyone have any comment on this workflow? Is there a simpler way?
Cheers
Think I've figured this out. Work flow for importing a Step assembly and creating a unified mesh of distinct volumes (eg. for different material properties), seems to be 1) Import .stp into Salome 2) Explode to Solids and Faces 3) Fuse Solids (multiple fuse operations are required to fuse multiple solids) 4) Partition the Fuse, using the faces from (2) to divide the body into individual solids (Partition the Fuse, then partition the subsequent partition to divide into multiple solids) 5) Explode the final partition into Solids and Faces 6) Mesh the (final) Partition 7) Define volume groups in the mesh based on the individual solids in the partition 8) Select faces for the boundary conditions from the faces exploded inside the partition.
This solved OK. Does anyone have any comment on this workflow? Is there a simpler way?
Cheers
Please Log in or Create an account to join the conversation.
- Joël Cugnoni
-
- Offline
- Moderator
-
16 years 6 months ago #1388
by Joël Cugnoni
Joël Cugnoni - a.k.a admin
www.caelinux.com
Replied by Joël Cugnoni on topic Re:Meshing Compsolid in Salome 3.2.2
Yes you are right, this is the \"traditionnal\" way of dealing with Assemblies in Salome.
An alternative could be to use special \"tie\" commands in Code-Aster to link the interfaces of each volumes. This solution may seem simpler to use, but it also has some drawbacks:
1) it adds a lot of equations to the system (lagrange multipliers)
2) the local stress field around the \"tied\" regions is inaccurte (but the global behaviour is correct).
To have an idea on how to define \"tied\" regions, you may have a look at the \"assembly\" example here:
www.caelinux.org/wiki/index.php/Doc:AdvancedExamples
(it is a bit outdated now , but the method & commands are still the same)
Regards,
Joël Cugnoni
An alternative could be to use special \"tie\" commands in Code-Aster to link the interfaces of each volumes. This solution may seem simpler to use, but it also has some drawbacks:
1) it adds a lot of equations to the system (lagrange multipliers)
2) the local stress field around the \"tied\" regions is inaccurte (but the global behaviour is correct).
To have an idea on how to define \"tied\" regions, you may have a look at the \"assembly\" example here:
www.caelinux.org/wiki/index.php/Doc:AdvancedExamples
(it is a bit outdated now , but the method & commands are still the same)
Regards,
Joël Cugnoni
Joël Cugnoni - a.k.a admin
www.caelinux.com
Please Log in or Create an account to join the conversation.
- Andy Foan
- Offline
- New Member
-
Less
More
- Posts: 16
- Thank you received: 0
16 years 1 month ago #1765
by Andy Foan
Replied by Andy Foan on topic Re:Meshing Compsolid in Salome 3.2.2
I'm a new user trying to evaluate and promote Salome-Mech, ie version 3.2.6, and I'm making progress. Problem is I'm stuck now because I can't work out how to solve a problem with an assembly of say two different materials. Your post is encouraging because obviously this can be done.
Can you explain in more detail with a simple example say two blocks of different material joined together and compressed between a fixed face at one end and a pressure at the other?
When you use the Code-Aster Wizard Linear Static method to generate the .comm file, how do you specify the two material properties? Or do you have to do it some other way?
Can you explain in more detail with a simple example say two blocks of different material joined together and compressed between a fixed face at one end and a pressure at the other?
When you use the Code-Aster Wizard Linear Static method to generate the .comm file, how do you specify the two material properties? Or do you have to do it some other way?
Please Log in or Create an account to join the conversation.
- Joël Cugnoni
-
- Offline
- Moderator
-
16 years 1 month ago #1770
by Joël Cugnoni
Joël Cugnoni - a.k.a admin
www.caelinux.com
Replied by Joël Cugnoni on topic Re:Meshing Compsolid in Salome 3.2.2
Hello,
to do this, you will need to edit the Command File (.comm) that the Wizard has generated for you: in Salome-Meca, right clic on the comm file and choose "Edit in Advanced command editor (EFICAS)".
Eficas is in French but you will probably be able to understand it however. Try to read the .comm file in a text editor too in order to understand its structure. By comparing with the "advanced examples" ( www.caelinux.com/CMS/index.php?option=co...;id=25&Itemid=40 )
you can start learning the syntax of the main commands.
To make it short, you will need to:
1) create groups of volumes for each material region in Salome
2) define several materials with the DEFI_MATERIAU command
3) assign materials to each region with the AFFE_MATERIAU command
Try to look at the assembly example in the "advanced example" section of the site. Note that these files ahve been generated with a previous version of Aster/Salome, but the general syntax should be nearly the same.
Good luck
Joël Cugnoni
PS: I will prepare a small tutorial on Eficas & the basic commands of Aster when I can find some time...
to do this, you will need to edit the Command File (.comm) that the Wizard has generated for you: in Salome-Meca, right clic on the comm file and choose "Edit in Advanced command editor (EFICAS)".
Eficas is in French but you will probably be able to understand it however. Try to read the .comm file in a text editor too in order to understand its structure. By comparing with the "advanced examples" ( www.caelinux.com/CMS/index.php?option=co...;id=25&Itemid=40 )
you can start learning the syntax of the main commands.
To make it short, you will need to:
1) create groups of volumes for each material region in Salome
2) define several materials with the DEFI_MATERIAU command
3) assign materials to each region with the AFFE_MATERIAU command
Try to look at the assembly example in the "advanced example" section of the site. Note that these files ahve been generated with a previous version of Aster/Salome, but the general syntax should be nearly the same.
Good luck
Joël Cugnoni
PS: I will prepare a small tutorial on Eficas & the basic commands of Aster when I can find some time...
Joël Cugnoni - a.k.a admin
www.caelinux.com
Please Log in or Create an account to join the conversation.
- Andy Foan
- Offline
- New Member
-
Less
More
- Posts: 16
- Thank you received: 0
16 years 1 month ago #1778
by Andy Foan
Replied by Andy Foan on topic Re:Meshing Compsolid in Salome 3.2.2
Got it working - to follow are the .hdf file and the .comm file before and after editing. Also a couple of pictures.
Thanks and Kind Regards
Andy
Post edited by: Andy Foan, at: 2008/02/28 00:56<br /><br />Post edited by: Andy Foan, at: 2008/02/28 00:57
Thanks and Kind Regards
Andy
Post edited by: Andy Foan, at: 2008/02/28 00:56<br /><br />Post edited by: Andy Foan, at: 2008/02/28 00:57
Please Log in or Create an account to join the conversation.
Moderators: catux
Time to create page: 0.130 seconds