matching mesh for structural non linear contact

  • 113 Views
  • Last Post 25 October 2018
DirtyCheese posted this 21 October 2018

Hi there,

i am trying to simulate a polygonic shaft hub connection with interference fit during load for 100 load cases.

I need to define a frictional contact between the shaft and hub. To accelerate the solving i want the nodes of the meshes on both faces to match exaclty. How can i controll this in ansys? The match mesh command doesn't do anything for me. Shared topology is only useful either ? What am i getting wrong?

Thank you in advance.

Best regards

Order By: Standard | Newest | Votes
peteroznewman posted this 21 October 2018

Hi DC,

The part you are getting wrong is the assumption that making the mesh on both faces match exactly is going to accelerate solving.  It's good to have similar sized elements on each side of the contact, but it's not a faster solve time for a frictional contact pair to have an exact match.

You don't want Shared Topology, that is useful for replacing Bonded Contact with shared nodes. In that case, there is no contact at all.

I found an image for a polygon interface. Is this the kind of shaft coupling you are working on?

Regards,
Peter

DirtyCheese posted this 21 October 2018

Hi Peter,

yes this the kind of connection i am working on.

I've been told that matching nodes espacially for the 1st step the interference fit, should be very numerical friendly. I know for sure that this function is implemented in other meshers . So i thought that this option should be available for sure in ANYS too.

peteroznewman posted this 21 October 2018

Hi DC,

The time it takes to solve frictional contact problems depends on the contact stiffness that is used and the amount of penetration that is acceptable in the solution. These parameters are available in the contact definition. In Analysis Settings, when Auto Time Stepping is On, there is some control over the Initial Substeps that can affect the overall solution time. If the number of substeps is too small, a bisection will occur, wasting all the previous iterations, if the number of initial substeps is too large, the solver will make more iterations than it needed.

If you want to Attach a Workbench Project Archive .wbpz file to your reply after you post it, I can reply with some mesh controls that give a good mesh on your bodies.

Regards,
Peter

DirtyCheese posted this 21 October 2018

Hi Peter,

i'm aware of this. I guess better control of the contact algorithm together with more efficient mesh should speed up the solving. Bisections dont occur the penetration was limited to a tenth of the interference fit. Tried pure penality and augmented penality. I'll come back to you tomorrow.

Can you tell me a work around to apply multiple remote forces on a common face without overconstraining it? I have two forces from different points in space.

Regards DC

peteroznewman posted this 21 October 2018

Hi DC,

Pure Penalty contact algorithm typically needs more iterations that Augmented Lagrange. There are many experts on this forum who might offer more detailed advice.

That's a good question about multiple remote forces on the same face. I don't think forces can cause an over-constraint. Displacements can cause over-constraint because a node can't be in two places at once, but it can be pulled in two directions at once.

Regards,
Peter

DirtyCheese posted this 22 October 2018

HI Peter,

i get the warning that my surface is overconstraint by multiple MPC. If I review the CE visually i see that 99% of my surface nodes are connected to one remote point and only a single node is connected to my 2nd remote point. I also want  to lock the rotation  of  a cylindircal surface around it's own axis whereas the surface should be able to deform and follow bending. I've done this by a remote displacement for this i also get a warning that i have a mpc resulting in a lot of CEs which may slow down the solution. Do you have any advice for me? 

The following article refers to my problem . From the ansys help i take that one can only adress one remote force and one moment to the same remote point

http://www.padtinc.com/blog/the-focus/donny-dont-remote-objects

Best regards,

DC

 

Edit: SInce i want a fast solution i think remote force is still better than modelling a rigid body. But what is the best practice in ANSYS for this

peteroznewman posted this 22 October 2018

Hi DC,

You say you get a warning that it is overconstrained, but isn't the warning that your model may be overconstrained? You can get rid of the warning if you exclude that single node from the scoping of the first remote point.  An image would help me understand what you are trying to do.

If you want to lock rotation of a cylindrical surface but allow bending, a remote displacement sounds like a good way to do that. You can limit the slow down by limiting the number of nodes that are included. For example, instead of selecting the cylindrical face, select the circular edge.

The Padt blog was referring to a model where a remote force and remote  moment were each individually created at the same remote location on the same face. This is wasteful because two remote points are created and two sets of CEs are created to the same surface. It's more efficient to create one remote point and one set of CEs then apply the two loads, a force and a moment to the remote point.

But if you have two remote points at different locations in space, you can't use that method, you need two remote points.

Regards,
Peter

DirtyCheese posted this 23 October 2018

Hi Peter,

doesnt that subsequently mean that the remote force is only "projected" on this single node?

 

This is my setup: i want both remote forces to act equally in the same time step on the same face. Subsequently i get the following message

If I refer to the troubleshooting no real solution to this problem is given.

The modell is currently solving I'll give you an update on the generated CEs when it's done.

I also want my meshnodes to match in the contact as well as the radial inflation layer direction of the elements to allign on both sides of the contact perpendicular to the surface they are originating from

Best regards 

DC

peteroznewman posted this 23 October 2018

That looks like a sweet mesh DC. It will be better with some radial inflation, as you said.

The force or moment is applied at the remote point. The spider of CEs transfer the load from the point to the face. As I said above, the warning is that the remote BCs may have conflicts, but in your case, with two forces, they are not in conflict.

Good luck with the solution. I hope you changed the Newton-Raphson Residual Plots from the default 0 to 3 or more. That will help diagnose any failure to converge.

Best regards,

Peter

DirtyCheese posted this 24 October 2018

Hi Peter,

thank you for your advice. I'll take ploting the Residual into account for my next calcuation. 
I forgot to take a screen of the CE's formed by the remote forces.
But I still don't know how to generate the mesh i am intending to achive within WB. 
Can you give me please some keywords or in detail description on this.
Thank you fo your advice.

Much apreciated!

Best regards,

DC

peteroznewman posted this 24 October 2018

Hi DC,

You want inflation on the shaft out to its outer contact surface.

I see you have sliced the part up. Are those parts Sweepable?  If you RMB on Mesh and Show Sweepable Bodies, do they light up green?  If so, you pick the 3 bodies and set the Method as Sweep and set the Source and pick the 3 faces and you can set the sweep number of divisions if you want. Then RMB on the Sweep mesh control and select Inflate this method. It already knows the faces, you just use the Edge filter and pick the three edges and fill out the inflation details.

Regards,
Peter

DirtyCheese posted this 24 October 2018

Hi Peter,

I'll try it this way right tomorrow ( UTC +1 here) thank you!

Best regards,

DC

DirtyCheese posted this 25 October 2018

Hi Peter,

since the the polygon shape is defined by a parametric curve generated in a non compatible CAD-licence. I have to import it as .stp and melt in SpaceClaim with the rest of my shaft. I guess in this CAD transition i lose some information of the curvature. i can't make the SpaceClaim equationgenerator make want i want him to do ;(. The polygon slices aren't directly sweepable but using multizone makes it look it's getting sweeped completly.It feels like Inflating a method has the same effect as choosing a inflation as a new operator - is this guess correct?
Still how can i force the mesher to mesh symmetric with matching nodes in a contact? The nodes in the following seem like being coincident but this is by coincidence I dont know why it worked out this time...

Best regards,
DC

peteroznewman posted this 25 October 2018

Hi DC,

If the bodies are not sweepable, Multizone includes an inflation option.

To get matching nodes on coincident edges, you can add a sizing control to both edges and specify the number of nodes on the coincident edge.

Regards,
Peter 

Close