Pro/Mechanica one-sided constraint? 1

[AHartman]

Hi all,

I have what I think is a simple question for using Pro/Mechanica. I'm modeling a vacuum chamber lid to see if it's likely to lose its seal under 1 atm of pressure. Is there a way to constrain the sealing surface so that it can't move in the negative Z direction, but can move in positive Z? That is, can I simulate the presence of the chamber's sealing face by telling Mechanica that the lid may deflect upwards (away from the chamber) but not downwards (interference with the chamber)?

-Adam

 

[seymours2571]

Adam,

Contacts are what you want to use. However, this will increase your solution time due to the introduction of non-linearities. Also, ensure you restrain all degrees of freedom (dof) with either constraints or contacts.

Also, I can't remember if contacts require the advanced Mechanica license or not.

Good luck,

Steve


Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com

 

[AHartman]

Steve,

Thanks for the heads-up on needing contact analysis. I've done my best to set on up, but I am somehow unable to get the constraints and contact interfaces to live together happily. Meshing never happens, with the error that my constrained surface is going to be deleted. I'm curious about this, since my interface is at the top of the lower plate, while the constrain is at the bottom of that plate.

Any advice?

Thanks in advance!
-Adam

 

[seymours2571]

Adam,

It sounds as if you are using mid-surface compression to model some sort of thin walled part. During the mid-surface compression proces to create the mid-surface shell elements the faces on the end will be "deleted". Thus, the error message associated with placing constraints on the end.

As an alternative if you want the constraints to be applied on the end just apply the constraint to the edge associated with the end face instead.

But you have a bigger issue at hand. Mechanica does not support contact with shell elements. This is a real disappointment given that other FEA programs do. If you want contacts you will have to model the problem using shell elements only...thus no mid-surface compression or explicit shell definitions.

Let me know if this is confusing and if I just muddied the water.

Thanks,

Steve


Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com

 

[AHartman]

Steve,

Thanks for your speedy response! I'm not doing a thin walled part per se...

thickness = 8 mm
length = 450 mm
width = 200 mm

Maybe that qualifies as thin walled, but doesn't feel like it to me.

I basically have a rectangular plate resting on top of a rectangular ring (the top "slice" of a vacuum chamber). Atmospheric pressure on the plate versus zero pressure in the chamber will deform the plate. I want to see if any gaps open between the plate and the ring.

Are you saying that I need to give up modeling the solid bodies and only model the shells instead? What's the right set of meshing options to get that? And, won't that not accurately reflect the stresses internal to the lid part?

Waters aren't muddled, but looking a bit murky for sure

-Adam

 

[seymours2571]

Adam,

Are you using mid-surface compression in your analysis? I assumed so based on the "constrained surface is going to be deleted" error response you were receiving.

Steve

Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com

 

[AHartman]

Steve,

The short answer is "I don't know..?"

I don't recall selecting that as an explicit option. How do I tell if that's being used? And, I guess, how do I know if I should be using it?

-Adam

 

[seymours2571]

Adam,

The easiest way would be to suppress all of you constraints and mesh the model using the AutGEM toolbar or menu option. If you have elements that show up as green you have shell elements present in your model.

To further determine if you are using mid-surface compression you will need to drill into the part or assembly and see if shells have been defined. The methodology differs somewhat between WF5 and WF1 thru WF4.
What version of WF are you using?

Steve


Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com

 

[AHartman]

Steve,

I'm using WF4. When I use the AutoGEM menu to mesh my assembly, only the first part is meshed. I do AutoGEM->Create->All with Properties, and it creates a nice tetra mesh of the first part in the assembly. The mesh info says no shells are created. It appears that I've got bigger problems indeed!

My methodology for making the 2nd (as of yet unmeshed) part was to take the full chamber, insert a datum plane about 5 mm below the sealing surface, then create a cut well outside the entire perimeter, "slicing" away all but the top sealing ring volume. When I try to just mesh this volume, individually, in the assy, I get an invalid selection message.

Is this the wrong way to create the 2nd part?

Thanks in advance for your continued indulgence

-Adam

 

[seymours2571]

Adam,

It sounds like you may not have material properties established on that 2nd part. Mechanica will not mesh parts without material properties defined within the context of the ProE assemlby.

From what I understand, I don't there is any problem with how you have created the geometry of your second part. This may also explain the error messages you were receiving. Because if the constraints are applied on a surface of a part that does not get meshed, then the constraints will essentially not exists. For constraints or loads to be valid they must be applied to bodies that are meshed.

Let me know if the material property definitions are or are not the problem.

Steve



Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com

 

[AHartman]

Steve,

To the best of my knowledge, the 2nd part is assigned material AL6061. When I try to just mesh the 2nd part in its own window, I get the error messge "The model does not have meshable geometry or idealizations"

Is it too complicated a shape? Maybe I have some mesh settings wrong and it can't complete a mesh with the parameters I've set?

-Adam

 

[seymours2571]

Hey Adam,

It sounds like you have a surface body for the 2nd part. If you change your display to wireframe are the edges all purple? If so it is a surface body. Then you will just need to solidfy the body in order for it to mesh in Mechanica.

Mechanica can handle some pretty seriously complicated shapes. I have meshed some pretty crazy geometry will hundreds of rounds and thousands of surface patches.

If you still have problems post the assembly to eng-tips and I will take a look.

Steve



Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com

 

[AHartman]

Steve,

When I turn on just wireframe, all the edges are white. Not sure if this can be changed or if it has been changed in some preference somewhere. Mass properties for the 2nd part reports a reasonable mass. When I try to do Edit->Solidify, the option is greyed out.

I'm pretty sure that it's got nothing to do w/ the slice operation that I did, because I can't mesh the parent part, either. Perhaps it is a good time to point out that the parts were made in SolidWorks 2009, then saved as ProE .prt files. Perhaps some conversion didn't work out so well?

I've attached the sliced part for your investigation. I'm not sure why the extension is .prt.11, but it's the most recent file, so I hope that's what you need. Again, thanks SO much for volunteering your time like this! It's always wonderful to learn from someone so generous!

-Adam

 

[seymours2571]

Adam,

Okay. Mecahnica appears to be having a beef with the geometry. It is strange because no "geom checks" appear within proE to indicate that there is a problem with the geoemtry.

However, what I did to get it to mesh was to make a surface copy of the entire sliced version of your model. Then I used a plain old extrude to cut away all of the solid model. Then I solidified the copied quilt surface. It was able to mesh that geometry. I have seen bizzar geometry issues before, however this one was pretty far up the list on the wierdness scale.

I have uploaded my version of the part so you can plow through the feature tree to discect what I did.

Let me know if this helps.

Thanks,

Steve

Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com

 

[AHartman]

Steve,

The mesh went fine, maybe. No errors from AutoGEM during a simple mesh creation. But, when I try to do the actual contact problem, I get an error saying it can't pair linked assembly elements near a highlighted feature. I've attached the screenshot to show you.

There are 4 red circles well away from the model volumes which I've circled in the image. Are these some sort of phantom elements/nodes which are making the mesher unhappy when it tries to do contact surfaces?

I set the Model Setup as default contact, all options checked and coefficient of friction 1.20. I then added a connection, contact type, with all options checked and the same coefficient of friction.

-Adam

 

[seymours2571]

Adam,

I am not sure what is going on with the 4 red circles. It appears that mechanical is seeing some geoemtry out in space that shouldn't be there.

Try posting the assembly file if you can and I will take a look at the whole thing. I think a lot of the errors you are experiencing have to do with the imported geometry not playing nice with Mechanica.

Steve


Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com

 

[AHartman]

Steve,

I've attached the assembly. I was pulled away onto other projects, so sorry if you felt like this thread dropped off the face of the earth!

-Adam

 

[seymours2571]

Hello Adam,

Okay...so I was able to get everything to mesh.

There were a couple of things going on. First, the two parts were mated together, which is fine, however Mechanica was having difficulty meshing the two parts because without a contact surface interface defined between the two parts Mechanical will bond the two parts using a conformal mesh between the adjacent boundaries. However, because the AutoGEM geometry tolerance was set to relative there were some edges and vertices that were being collapsed in order to simplify the mesh. This simplification was resulting in degenerate geometry at the mated surface between the two parts.

Setting the AutoGEM geometry tolerance to Absolute helped somewhat, but still resulted in errors. The mesh size ballooned due to many of small edges, surfaces, and vertices that were now being included in the geometry model during meshing. However, a single pass complete mesh could not be generated and Mechanica could not complete the mesh on subsequent passes.

However....having said all of that...the ultimate solution was to leave the AutoGEM geometry tolerance setting to Relative and create a contact interface between the two mated parts. This was not present in your model. By creating this contact interface between the two parts mated surfaces will be treated as separate by the mesher. Therefore, there will not be a conformal mesh created across the mated boundaries of the two parts.

I also notices that there was a fixed displacement constraint applied on the mating surface between the two parts. This will need to be removed as well prior to running a contact simulation as the fixed displacement constraint would conflict with the contact surfaces. You could place the fixed constraint on the opposite side to prevent any rigid body motion during the simulation.

Keep in mind with the fine mesh controls specified (i.e. 6 mm according to the model) this contact simulation will take some time. Also, don't forget to add either more contacts or constraints to all of the parts to prevent any rigid body motion, especially rigid body motion within the plane of contact between the two parts.

Let me know if you still have issues.

Thanks,

Steve



Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com