fatal error E5000

[Anonymous]

Hello everyone,

I am performing an Linear Static analysis for a bus prototype which contains lots of big and small parts with different materials. After running the simulation I am not getting any warning only a Fatal error E5000 (Singularity detected). I have tried various solutions as mentioned in forum like:

1. Check material properties

2. Run the simulation with modal analysis to find out the distorted part (distorted part should be highligted in colour but I am not getting any coloured area.) 

3. Remove the value of G from the properties.

i have tried all these ways but couldnt avoid E5000. I am using  mostly aluminium and steel as the materials but there is one rubber material is also used with low youngs modulus resulting lower value of G. Is it the one which is causing the Error? I am not pretty sure. If yes, how could i proceed without removing that material?

Thank you

[KubliJ]

Hi @Anonymous 

Are you using any surface contacts? I ask because the modal analysis will turn all separation contact into bonded. So if you have any parts that are held in by place by separation contact, you wont be able to identify it with a modal analysis.

Are there any other warnings?

Thanks,

James

[Anonymous]

Hi @KubliJ,

Thanks for your reply, as there are too many parts i have created the contacts through solver contact (bonded contact).

luckily I am not getting any warnig accept Error E5000 (Singularity detected). Material properties are ok, there might be slight collision between the parts (Please see the attachment). could it also be a reason of this Error? Can mesh refining help? Its quite frustrating now i have been stuck here for 3 days. please suggest me something.

thank you

[Anonymous]

Hi @KubliJ ,

If this attachment could help to get some idea.

Thank you

[Anonymous]

Hello @KubliJ ,

I have checked all the parts and assemblies if there is some unconstrained contacts. I have also removed the collision between the parts but still getting the error. When I choose DECOMPMETHOD to AUTO I get fatal error E5000 and when I choose PCGLSS I get E5004.

thank you

[Anonymous]

Hi @KubliJ,

i have removealmmost all the interferences, there are some hair line interferences left which are very difficult to remove. Is it ok if i leave them or should i try to remove them too? Please suggest somthing.

Thank you

[KubliJ]

Hi @Anonymous,

Sorry for the delay, yesterday was a little busy. I've had a chance to review the model.... there are a lot of things to discuss. In short though, this model is too complex 'as is' to perform a simulation on.

The structure has lots of gaps that I assume will be closed by welding together. This is going to cause problems for the analysis. The contact will have to be manually defined. Or you can use the solver contact, but that is global and may have other issues.

As you mentioned, there is some interference in the model that is going to cause issues with connecting parts. Here is an example I found in the frame:

There are some free floating parts. Some washers and other things I couldn't identify. There are some parts that only contact on an edge, which will cause them to behave like a hinge on that edge and freely rotate.

And there is also some very small features (bolt holes) compared to the overall size of the model that make things difficult for the mesher.

Speaking of meshing, how did you get the model to mesh? I took one sub assembly and tried to mesh it as a solid. It failed to mesh everything and in trying to get things to work ended up with a mesh of over 6 million elements. And this was just for a sub assembly.

I tried using the midplane (Find thin bodies) but that tool is having difficulty with some of the features. In the screenshot below you can see how that forked shaped body is converted to a surface part:

I think this model needs to be rebuilt into a simulation specific model as it is too large and complex to function. I'm going to create a little video show how I would rebuild the model, but I am doing it on one of the smaller subassemblies as it is a lot of work and would probably take many hours to do for the full model.

I'll link the video in my next post.

Thanks,

James Kubli, P.E.

Edited... fixed some grammar.

[KubliJ]

Here is the sample video I promised on how best to modify the model.

https://autode.sk/2O7PmqN

[KubliJ]

I try to take on a bigger section. Spend over an hour modifying the model just to end in failure. You can give it a watch to see what strategies I take....

https://autode.sk/2RUEr53

Thanks,

James Kubli, P.E.

[Anonymous]

hi @KubliJ ,

Thank you so much for your effort. i will change the model and let you know how it went with simulation.

Thank you

[Anonymous]

Hello @KubliJ ,

As you have advised I have simplified the model as much as possible I have also removed all the small chamfer and the fillets, I am not getting any error ore warning now, I have meshed it too but after the simulation is run I am getting very high values of stress and displacement(in millions). I have just found the high value I am getting is due to the addhessive material used between some metallic surfaces to glue them. The values of the addhesive material is very low hence reduceing the stiffness of the model. But the addhesives are  necessary part of the model that I am not supposed to remove. I am bit confused what can I do now is there any alternative? or any other way you want to suggest.

Thank you

Anurag

Anurag

[John_Holtz · Accepted solution]

Hi @Anonymous 

As you have discovered, the ratio of large stiffness (probably steel, but I have not looked at the model) and weak stiffness (adhesive) is a problem with producing accurate results. 

I think these are your options:

• Include the adhesive and do not get results.
• Remove the adhesive and get results.
• Include the adhesive but make the material properties stronger until you get realistic results.

Note that I am assuming that the mesh is fine enough to not be part of the problem. One of your other posts showed that you have very thin parts and very large solid elements. The distortion of the solid elements because they are so thin can be enough to cause solution problems in some model. (Any shape that is not an ideal 4-node pyramid can cause a problem.) You might want to consider using shell elements for the thin parts of the model.