Learning Forum

[ritesh singh]

hello guys. i have been trying FEM of Wire arc additive manufacutring process ( layer is deposited on substarte plate) a type of additive manufacturing process. In my model, square layer is deposited on substrate. I have used coupled transient thermal and transient structural analysis module. Bilinear isotropic hardening model is used as plasticity model. my thermal simulation is giving results but during structural analysis it is showing non convergence error. i have tried it with smaller mesh size but it is still showing same error.
I have completed the simulation for 16 layers straight wall using same material properties and analysis setting and mesh even larger than the current one, but for square deposition it is showing non convergence issue. 

kindly help me through this problem. i have been stuck on this from last 1 month.
i have attached the images of, mesh, structural analysis setting, thermal analysis setting, material properties and error to the post                                                            

 

[mjmiddle]

Please select the "Solution Information" and scroll up to the last error.

[ritesh singh]

thank you for reply. i have attcahed the img of last error shown in it.

kindly ley me know any method to solve this error.

[mjmiddle]

Try setting a nonzero Newton Raphson Residual:

After it fails you can view these problem locations under the Solution Information Outline object.

[mjmiddle]

You can try setting smaller time stepping, especially initial time step if if has not converged one substep. If it can can converge a few substeps, set a smaller minimum time step.

[ritesh singh]

i have used these values for analysis setting in structural as well as in thermal. and still it is showing convergence error. i have attached image of error from solver output. kindly help

[mjmiddle]

What is that structure pusing up though the plate? Are there some geometry features inside the plate? Can you show a section plane through that region? And show some mesh. You can hide some outside faces also to see inside the model. What are the loading and supports on this model? What is it doing in load step 2? Your first picture showed it was on load step 2, so it must have converged load step 1. What is being done in each load step?

A maximum of 5 substeps is not much to allow. Try initial substeps of 100 or 1000, and maximum substeps 1e4 or even 1e5. The auto time stepping can adjust the times higher if it starts converging easier. Let it run overnight. If you get any converged substeps, you can look at deformation and stress results to see what it's doing. Or rather than let it run a long time, if it converges a few subteps, but looking to take more iterations to the point you think it's eventually going to fail, then you can interrupt and look at the results of the few converged substeps to see how the model is behaving.

[ritesh singh]

that pushing up structure should not be there. the model consist of solid plate on which sigle layer square deposition is made. i have given frictionless support to outer and inner faces of square layer and fixed supoort to a node at lower face of plate. this support conditions i have tried on straight wall deposition also, and it worked for that. and in each load step, basically each side of square is being deposited.  

[mjmiddle]

I see now that image was a deformation result. I had assumed it was a Newton Rapshon residual, because that was what I asked you to send. The max is very small at 6.9094e-5m, so you must be showing a highly scaled result. That pushing-up structure is just some minor movement of nodes. View it in true scale.

With a non-linear contact like frictionless support holding the inner square, you will certainly need small time steps. Try the substepping I suggested in my previous post.

In addition, if you are expecting the fixed support on one node to prevent rigid body motion, this is not enough. It will prevent translaations, but not rotations. You will need to apply to 3 non-colinear points to prevent rotations, and thoroughly fix the model from rigid body motion. If you only apply to 2 nodes, then the model can still rotate around the axis that goes through both points. That is why you need 3 non-colinear vertices or nodes for the fixed support. Or another way to do this is to apply a remote displacement of zero translations and rotations to a face, and make sure to set to deformable behavior. This is the better method if you want that entire both to be deformable yet not move in rigid body mode.

[ritesh singh]

 

thanks for the reply. i have tried the model with coarser grain struture of 4mm hexahedral element and as shown in attached image. it is showing results. but when i increase heat input from 300 to 838, it is again showing convergence error. At heat input of 300, peak temp is reaching 960 C approx. At heat input of 838 peak temperature reaching is approx 3000 C (although it is 800 C greater than expected), for the same mesh arrangement. kindly help. (its been 4 months since i am working on this convergence issues). all the boundary conditions and the materials are same as in previous posts.

 

[mjmiddle]

The discussion and pictures have all been about a structiral model so far. You lastest post descibes a heat input and temperature output, which is a different analysis, so I assume you have a one-way thermal analysis linkage into this structural model. I don't know if your time stepping of 640 sec load step, 16 s intital, 12.8 s min, 64 s max are for the thermal or structural analysis. For a structural analysis, this means only a max of 50 substeps. In a problem model, you can allow for a lot more substeps, like 1e5. This would be a 0.0064 minimum time step. The auto time stepping can adjust larger when time stepping is easier.

[ritesh singh]

Yes. it is coupled transient thermal-transient strutural model. And i have used same time stepping for for both the analysis. and it has given me the results for heat input of 300. but for same meshing and analysis setting it is giving convergence error when i increased the heat input to 838. kindly help.

 

[mjmiddle]

Be aware of the warnings and errors during the iterations if it has many time bisections and doesn't appear to be converging. Also, view nwnton raphson residuals for problem locations.

[ritesh singh]

thank you for your suggestions sir. i have a doubt. since model attached to the above question has run on the above mentioned transient structural and thermal analysis settings (as attached in images). i thought that it will run for larger heat input also. but it is showing convergence error of highly distorted elements. As you suggested to decrease time step, does this mean that meshing and other analysis parameter depends on heat input that i am giving? if i have run a model on particular settings and meshing, do i have to change it if i am increasing heat input?

[mjmiddle]

The magnitude value of your loads can certainly affect convergence. Small loads are generally easier to converge. Mesh size can certainly affect convergence also. A minimum time step that would only allow 50 total substeps is not much in a model that's having problems converging. I would only have such settings in a model that runs easily. With highly distorted elements, the model probably has some ill conditioning, and small time steps can somtimes overcome this, but there are probably some more core problems in the model. It may be material properties. It may be connections. The Newton Rapshon residuals help show the problem locations. Transient structural analysis can have a hard time running when there are significant forces/accelerations in small gaps, so that parts "chatter." You usually need to add some damping either globally, or more locally through material definition or damping on a spring or revolute joint.

[mjmiddle]

I noticed 1-2 elements across thin body thickness. Try more, like 3-4.