FATAL ERROR T2144 in Impact Analysis

[mwighton]

Im trying to run an impact analysis that consists of 2 blocks hitting each other. Both are Aluminum 6061 with a symmetric separation contact between them.

As per the help files, "If using shell elements make sure the projectile element normals are facing the body and vice versa." only problem is I am not using a shell element, so I am not sure what to do to fix this issue.

[John_Holtz]

Hi @mwighton

I just tried a sample Impact Analysis, and I was getting two errors:

• T2135 Unable to generate surface contact using specified parameters
• T2144 Unable to generate impact analysis parameters, status 4

The "status 4" is really the same problem as the T2135 error, and one solution (as you mentioned) is related to the shell element orientation. That is obviously not the problem in your model.

This is just a guess based on the problem I encountered and the solution. The documentation for the Impact Analysis is not real clear, but I think the projectile path (sketch line) needs these two requirements:

1. The path must start at the projectile and end at the impacting surface. (I started my sketch from a corner of my projectile, but I gave it an arbitrary length to give the direction. It was passing through my impacting surface.)
2. There needs to be a node on the projectile and impacting surface at the end of the sketch path. You can do this by using the "Mesh Control" and adding the end points of the path sketch line.  See the attached sketch. (I only needed to end one end because I started the path from a corner of the projectile which will have a node.)

Let me know if this is the solution for you, and I will write-up an article.

[Edit] You do not need to define the contact surfaces. The impact analysis figures that out, presumably by having a node at each end of the projectile sketch path.

[mwighton]

During my initial setup of the problem I had already made my projectile path from surface to surface and created a corresponding mesh so that each point was at a node.

[John_Holtz]

Hi,

There is one other suggestion that I came across. See Fatal Error T2135 when running impact analysis

If that is not the solution to your problem, would you be able to zip (compress) your assembly and part files and attach it to a reply?

[mwighton]

I initially had the contact tolerance in the impact setup as AUTO. I just changed it and put a value that made sense for my model, but I still get the same fatal error.

Unfortunately I can not send a file.

Any other ideas as to why I am getting this error?

[mwighton]

Hi John,

So I did some searching and found a post on the forum for a solution to FATAL ERROR T2135 (which you said is the same issue in my case) and although the solution was not explicit the general idea was that the issue was stemming from a constraint or contact. So.... I changed my separation contact from a manual selection between the two surfaces that would interact and made it an automatic contact, selecting the two bodies that will interact. The analysis seems to be solving now. Can you try this on your model and see if this works as a solution? If it does, this is something to look into about the solver issues.

[John_Holtz · Accepted solution]

Hi M,

This is just a guess on my part, but I think that if you define the contact as "Manual" and pick the "Master" and "Slave" surfaces, this will create contact between those surfaces first. When the Impact Analysis tries to create the contact between those same surfaces later, it cannot do create the contact (because it already exists? because it does not want to overwrite something the user created?) and gives the warning and error.

If you define the contact using "Auto", and either select the surfaces or do not select the surfaces, my guess is that the Impact Analysis creates its contact first, and then the Auto contact creates other contacts second, but it does not complain that a contact is already defined.

But you do not need to define any contact for the impact. That is done by the Impact Analysis and is why the projectile path needs to connect from a surface on the projectile to a surface on the impacted.

[oleg.cmg]

Hi!

I'm have same problem too.

I can't solve simple drop test. What's wrong?

[John_Holtz]

Hi @oleg.cmg Welcome to the In-CAD forum.

I took a look at your model. I do not know what's wrong with it.

I wonder if it will work if the projectile is at a different angle compared to the floor? I will continue to look at it.

[oleg.cmg]

Hi John!

I Think i have solution for this trouble....

The projectile part is too far from grounded part.

I move projectile part to ground part. After that Nastran solved this task.