Negative Volume Err...
 
Notifications
Clear all

[Solved] Negative Volume Error (following LS-Dyna Tutorial)

5 Posts
3 Users
3 Likes
5,388 Views
Posts: 6
Topic starter
(@auburnaudi)
Student
Joined: 3 years ago

Hi all,

I am very new to LS-Dyna (but am familiar with other FEA software/solvers - such as Hypermesh) and have started by following along with tutorials and other examples to get the hang of it. I am currently working through the "LS-Dyna Ball and Block" tutorial on YouTube by the channel Unpopular Mechanics (part 2 here: https://youtu.be/QwR43Arank0 ). I am fairly certain I followed every step and input exactly as described in the tutorial videos, but when I attempt to run the file to obtain results, I am met with a "negative volume in solid element" error and it terminates. (My animation with the d3plot looks nothing like what is then shown in the YouTube video - it is cut short at only 9 frames.) I have looked through some other posts in this forum about negative volume errors but was unable to find anything useful for my situtation, so am posting this in the hopes someone may have some helpful pointers.

My questions are then:

- has anyone tried this same tutorial and had this same error that causes the simulation to end prematurely?

- what does the "negative volume" error mean? Is there something that can be modified in the material or element properties that could help with resolving this error?

Thank you in advance for any insight you can provide. I really appreciate any help.

4 Replies




Posts: 3
(@farshid-er)
Barista
Joined: 3 years ago

Hey there,

 

I did not watch the tutorial, but I remember once I had the same problem, "negative volume". It happens when the deformation for an element is so severe that the solver cannot calculate its volume correctly. If you open the d3plot file, you should be able to find that element and see it for yourself. Also, I remember that the error would state the number of the element.

However, there are some things you can do about it. First, check if you are using the same version of solver as the tutorial. Then, you can look for changing the time scale factor in CONTROL_TIMESTEP keyword. Besides, changing section for solid elements can help to resolve this. As far as I know, constant pressure elements in SECTION_SOLID keyword is the most stable one. Overall, if you check the d3plot in LS-PrePost, I think you can figure it where the problem is.

I hope this helps you.

 

Reply
1 Reply
(@auburnaudi)
Joined: 3 years ago

Student
Posts: 6

@farshid-er

Thank you for your response! The information about "negative volume" is helpful.

I am pretty certain I am not using the same version of solver as the tutorial (it doesn't actually show the solver, just LS-PrePost, but I am using a different version there as well). I have modified the CONTROL_TIMESTEP keyword and have confirmed that I am using constant pressure elements in SECTION_SOLID for the block (the ball uses SECTION_SHELL defaults) but am still running into what looks to be the same negative volume error so I will need to look at the d3plot some more and do a bit more troubleshooting.

Thank you for your pointers!

Reply




Posts: 6
Topic starter
(@auburnaudi)
Student
Joined: 3 years ago

I haven't updated this topic in a while, but I was able to solve this negative volume error!

I gathered the following tips from a number of different sources and a couple of other forums and thought I would provide them here in case they can help someone else with this error (these are what I used in the tutorial model, as well as other models in which I received the same error / in order to avoid the error):
- Negative volume will cause the solver to terminate unless (1) ERODE = 1 in *CONTROL_TIMESTEP and (2) DTMIN =/= 0 in *CONTROL_TERMINATION.
- I am working with high strain rates, so I reduced the time scale factor (TSSFAC) in *CONTROL_TERMINATION from the default 0.9 to 0.667.
- For ELFORM, avoid fully integrated solids (formulations 2 & 3) and use 1-pt for large distortions. I ended up going with ELFORM = 10 (1-pt tetrahedron) since I eventually replaced the block with geometry that would undergo large strains and I had meshed with tetrahedrons.

I also saw some suggestions of checking units, stiffening the material stress-strain curve and further tailoring the mesh.

Hope this helps!

Reply
1 Reply
(@haider-mraih)
Joined: 5 months ago

Barista
Posts: 1

@auburnaudi Thanks so much; your comments helped me.

Reply







Share: