Space debris capture simulation issue

[Sahasra Boyapati]

Hello everyone, 

I am working on a space debris capture simulation using kevlar net. When I run the simulation, the net either disappears or does not even show up in the post process. The following are all the parameters i have on the net, I am also attaching the key file for reference. If anyone can guide me on how to fix this issue, i would really appreciate it. 

Net: 

• Size: 10cm x 10cm
• Thickness of the kevlar thread: 1.1mm
• Mesh: 2D tria shell elements
• The net needs to move towards the debris, capture it and wrap around it. 
• Material model: MAT_58_LAMINATED_COMPOSITE_FABRIC
• Section shell card: ELFORM = 16 (fully integrated shell element)

Debris:

• Size: 4cm in diameter, sphere shape
• Mesh: 3D tetra elements
• Solid rigid body and is fixed in all directions
• Material model: MAT_20_RIGID
• Section solid card: ELFORM = 1 (constant stress solid)

Velocity: INITIAL_VELOCITY_GENERATION = 4.5m/s

Contact parameter: CONTACT_AUTOMATIC_SURFACE_TO_SURFACE

I also activated CONTROL_TERMINATION, CONTROL_TIMESTEP, CONTROL_ENERGY, and DATABASE_BINARY_D3PLOT cards too. 

I do not see any errors and it says normal termination, but I cannot see the net moving closer or in fact doing anything other than disappearing or staying in the same place. 

I really appreciate if anyone can help me with this, I have been trying to make this work for a couple of weeks. Thank you so much! 

[James Kennedy]

Dear Sahasra,

 

Please check to make sure that you are using a consistent set of units for the different materials.

 

https://lsdyna.ansys.com/consistent-units/

 

A mass density of 0.00281 (rigid material) usually refers to specific high-strength aluminum alloys

when measured in grams per cubic millimeter (\(g/mm^3\))

 

The Young’s modulus for aluminum appears to be 71,700 Mega-Pascals.

 

You have indicated that the initial velocity being applied is 4.5 meters/second.

 

These units appear to be inconsistent.

 

Sincerely,

James M. Kennedy

KBS2 Inc.

May 11, 2026

--
You received this message because you are subscribed to the Google Groups "LS-DYNA2" group.
To unsubscribe from this group and stop receiving emails from it, send an email to ls-dyna2+u...@googlegroups.com.
To view this discussion visit https://groups.google.com/d/msgid/ls-dyna2/98a29123-9bd2-4920-afee-21ad3db090d6n%40googlegroups.com.

[Sahasra Boyapati]

Hello,

The units of the model are in mm, ms, g and N. So i have all the values in g/mm^3, MPa and for the velocity its in mm/ms which cancels out and we get m/s. 

[Ameen Topa]

Dear Sahasra,

You are using MAT058 for the net, which is modeled as solid elements. This is an interesting choice of material. 

From my experience, sudden disappearance in the elements as soon as the simulation starts could be due to improper material constants for composite materials. To make sure this is the issue, try running the model with MAT ELASTIC for the net and if the problem is solved, then we can know for sure that something is wrong with the material model. 

Regards,

Ameen

To view this discussion visit https://groups.google.com/d/msgid/ls-dyna2/CAL7VbM%2BwW%2BUdv7jk12EcoEqh3H7qB0y__1Oy_LBPxOru_wqTzg%40mail.gmail.com.

[Sahasra Boyapati]

Hello,

Correct me if i am wrong, Isn't 2D tria elements shell? I used the 2D mesh for the net and the mock debris is tetra solid. I will try the MAT_ELASTIC and see how that goes. Thank you!

[l...@schwer.net]

Ameen provided good advice.

 

One of your  *MAT_LAMINATED_COMPOSITE_FABRIC parameters, i.e. TSIZE=1.1, is the time increment above which the element should be deleted. Since your default time increment is 6.70E+03, all the elements of your “net” were deleted before the first time step.

 

Also, your initial time increment needs to satisfy the minimum time increment for the contact algorithm, as specified in the d3hsp file of

8.886E-05

 

I will send you the input file I modified.    --len

To view this discussion visit https://groups.google.com/d/msgid/ls-dyna2/b1bebe2b-a425-482a-b0e0-50fc544cacden%40googlegroups.com.

[James Kennedy]

 

In general, to build a 2D model for simulation as opposed to a 3D simulation in LS-DYNA, you simply

need to construct your model geometry in the x-y plane and use the 2D element formulation options

provided on the *SECTION_BEAM (plane or axisymmetric shell) and/or the *SECTION_SHELL (plane

or axisymmetric solid) entries, plus be geometrically correct with respect to the nodal loads, *LOAD_

NODE and *LOAD_SEGMENT_xxxx, entries.

 

From: ls-d...@googlegroups.com [mailto:ls-d...@googlegroups.com] On Behalf Of Sahasra Boyapati

Sent: Tuesday, May 12, 2026 11:26 AM
To: LS-DYNA2 <ls-d...@googlegroups.com>

To view this discussion visit https://groups.google.com/d/msgid/ls-dyna2/b1bebe2b-a425-482a-b0e0-50fc544cacden%40googlegroups.com.

[James Kennedy]

Dear Sahasra,

 

Something that might be of some interest.:

 

Reid, J.D., Lechtenberg, K.A., and Stolle, C.S., "Development of Advanced Finite Element

Material Models for Cable Barrier Wire Rope", MATC-UNL: 220, Mid-America Transportation

Center , TRP-03-223-10, Midwest Roadside Safety Facility, Lincoln , Nebraska , August, 2010.

 

http://ne-ltap.unl.edu/Documents/NDOR/advance_finite_element_models.pdf

 

Stolle, C.S., Reid, J.D., and Lechtenberg, K.A., "Development of Advanced Finite Element

Material Models for Cable Barrier Wire Rope", TRP-03-233-10, Midwest Roadside Safety

Facility, Lincoln , Nebraska , May, 2012.

 

http://mwrsf.unl.edu/researchhub/files/Report42/TRP-03-233-10%20%28MATC-UNL-220%29.pdf

 

Stolle, C.S., and Reid, J.D., "Modeling Wire Rope Used in Cable Barrier Systems", 11th

International LS-DYNA Users Conference, Dearborn , Michigan , June, 2010.

 

http://www.dynalook.com/international-conf-2010/Simulation-4-1.pdf

 

Judge, R., Yang, Z., Jones, S.W., and Beattie, G., "Numerical Simulation of Spiral-Strand

Cables Subjected to High Velocity Fragment Impact", 8th European LS-DYNA Users

Conference, Strasbourg , France , May, 2011.

 

http://www.dynamore.de/de/download/papers/konferenz11/papers/session18-paper-2.pdf

 

Bielenberg, R.W., Stolle, C.S., and Reid, J.D., "Improved Models of Cable-to-Post Attachments

for High-Tension Cable Barriers", TRP-03-267-12, Midwest Roadside Safety Facility, Lincoln ,

Nebraska , May, 2012.

 

http://ne-ltap.unl.edu/Documents/NDOR/Cable-to-Post_Attachments.pdf

http://nlcs1.nlc.state.ne.us/epubs/R6000/B016.0190-2012.pdf

 

Bateman, R.J., Faller, R.K., Bielenberg, R.W., Sicking, D.L., Reid, J.D., Stolle, C.S., Lechtenberg,

K.A., and Rosenbaugh, S.K., "Design of Cable-to-Post Attachments for Use in a Non-Proprietary,

High-Tension, Cable Median Barrier", TRP-03-285-13, Midwest Roadside Safety Facility, Lincoln ,

Nebraska , August, 2013.

 

http://www.transportation.nebraska.gov/mat-n-tests/research/docs/DesignofCabletoPostAttachments.pdf

 

Stolle, C.S and Reid, J.D., "Development of a Wire Rope Model for Cable Guardrail Simulation",

International Journal of Crashworthiness, Vol. 16, Issue 3, pp.331-341, 2011.

 

http://www.tandfonline.com/doi/full/10.1080/13588265.2011.586609#.UmEz0RDjeVo

 

Stolle, C.S., "A Concise Model of 3x7 Wire Rope Used in Cable Guardrail Systems", Master's Thesis,

Department of Mechanical (and Materials) Engineering, University of Nebraska-Lincoln, Lincoln,

Nebraska, May, 2010.

 

http://digitalcommons.unl.edu/cgi/viewcontent.cgi?article=1007&context=mechengdiss

 

Stolle, C.S., "Cable Median Barrier Failure Analysis and Remediation", Ph.D. Thesis, Department

of Civil  Engineering, University of Nebraska- Lincoln, Lincoln , Nebraska , December, 2012.

 

http://digitalcommons.unl.edu/cgi/viewcontent.cgi?article=1056&context=civilengdiss

 

Sincerely,

James M. Kennedy

KBS2 Inc.

May 14, 2026

 

 

From: l...@schwer.net [mailto:l...@schwer.net]
Sent: Tuesday, May 12, 2026 3:01 PM
To: 'Sahasra Boyapati' <mintub...@gmail.com>
Subject: RE: [LS-DYNA2] Space debris capture simulation issue

 

I think you want something that acts like a cable, i.e. minimal bending stiffness – truss elements.

 

Have a look here to see if anyone has modeled cables:

 

The web site:  LSDYNA Conference Papers

provides access to most of the LS-DYNA Conference manuscripts (PDF files).

 

From: Sahasra Boyapati <mintub...@gmail.com>
Sent: Tuesday, May 12, 2026 12:55 PM
To: L...@schwer.net
Subject: Re: [LS-DYNA2] Space debris capture simulation issue

 

mat58 is basically for composite fabric. I also tried  MAT001_ELASTIC, and I still see the bouncing of the net upon contact. Based on your experience, what material model would be ideal to capture a kevlar net wrap around a debris? 

 

On Tue, May 12, 2026 at 3:12 PM <l...@schwer.net> wrote:

Sound like an “elastic” collision.

Could be your net material is too stiff?

I know nothing about MAT058.

 

From: Sahasra Boyapati <mintub...@gmail.com>
Sent: Tuesday, May 12, 2026 11:45 AM
To: L...@schwer.net
Subject: Re: [LS-DYNA2] Space debris capture simulation issue

 

Hello,

 

I ran the file but the net keeps bouncing back after contact. Do I need to give additional contact input such as CONTROL_SINGLE_SURFACE to make the net wrap around the mock debris object? Or do I need to do anything else? 

 

On Tue, May 12, 2026 at 1:47 PM <l...@schwer.net> wrote:

See time increment related modification in this input file.        --len

 

From: ls-d...@googlegroups.com <ls-d...@googlegroups.com> On Behalf Of Sahasra Boyapati
Sent: Tuesday, May 12, 2026 9:22 AM
To: LS-DYNA2 <ls-d...@googlegroups.com>
Subject: Re: [LS-DYNA2] Space debris capture simulation issue

 

Hello,

 

Correct me if i am wrong, Isn't 2D tria elements shell? I used the 2D mesh for the net and the mock debris is tetra solid. I will try the MAT_ELASTIC and see how that goes. Thank you!

 

On Monday, May 11, 2026 at 6:31:19 PM UTC-4 engine...@gmail.com wrote:

To view this discussion visit https://groups.google.com/d/msgid/ls-dyna2/78cd0a3f-eff7-4763-8077-7879a731b792n%40googlegroups.com.