Can I use density in kg/mm3 instead of tonne/mm3 in explicit dynamic analysis model in Abaqus/CAE

[mgj2015]

Hi all,

I am using Abaqus/Cae to create needle-rubber interaction analysis. Every time when I used the material property density in tonne/mm3, the simulation fails because of material failure and come out as error. When I change the density to kg/mm3 the models runs through with convergence and no error in running.

Can some one please help me out. I am using steel properties for needle. If I use 7.8e-6 kg/mm3 instead of 7.8e-9 tonne/mm3 for material density would it make any difference in the final results of the model. If yes how can I solve the issue.

As I don't see any difference in unit conversion if I use kg instead of tonne.

Kind regards
MGJ

 

[ThomasH]

Hi

Since I don't use ABAQUS I can't really be sure but, I think you can use any unit system as long as it is consistent. So you can not just change the density but also the other parameters that are effected. You can find some exempes on consistent unit systems here:

https://femci.gsfc.nasa.gov/units/index.html

My guess is that what you are doing is actually something called mass scaling. By adding nonphysical mass to the system you increase the timestep and that makes the analysis run. Info on mass scaling:

http://www.dynasupport.com/howtos/general/mass-scaling

Good Luck

Thomas

 

[IRstuff]

For that matter, why not use 7.8 gm/cc or 7800 kg/m^3, both of which are more standard representations?


TTFN
I can do absolutely anything. I'm an expert!
faq731-376 forum1529

 

[mgj2015]

Thanks Guys,

If I use the consistent scaling in si or metric, the models runs as failure due to element distortion. I guess the answer lies in mass scaling. I will look into that, and get back to you guys.

 

[IRstuff]

The notion of a nano-tonne as a mass just seems really bizarre to me, but even a micro-kilogram is almost as odd.

TTFN
I can do absolutely anything. I'm an expert!
faq731-376 forum1529

 

[IceBreakerSours]

Since you brought up mass scaling, I have a question for you: Are you using double precision for your explicit job? And, by the way, what's the reason for choosing explicit? Can you talk briefly about the phenomenon you are trying to model?

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[mgj2015]

Hi Ice

I am trying to stimulate the puncture of rubber through needle. I can't use static standard model as I am looking to analyse the needle puncture through the rubber by ALE eularian analysis. As I am trying to create deformation in rubber with material motion rather then element deletion model. I know I can run element deletion model but it won't give me true design method to see the force acting on needle. I am trying to see the Force displacement model in needle with experiment setup. No I am not using double precision as it is not needed. I have the model of needle which is in less then .5 mm diameter internally and .7 mm outer as u can imagine .1 mm thick. So I have very fine mesh and that's the reason I need to use mass scaling probably bcoz the element at the tip fails if I don't use mass scaling of those elements which come in contact with rubber while cutting through it.

 

[Dave442]

If your model fails when you assign consistent units then there is a problem with your model. Although adjusting the density of your material seems to allow your analysis to complete, you are scaling the mass of your material by three orders of magnitude for no reason - that is significant. Are you sure you have assigned consistent units for all of your geometries/loads? As your density is in tonne/mm then your length = mm, force = N and pressure = MPa etc... Also, why is double precision not needed? If you have a large number of elements in your fine mesh you may require double precision as suggested above. You should get a warning in the .sta file.

 

[mgj2015]

Hi Dave,

My models runs without any failure in element distortion if I use the density in kg/mm3 rather then tonne/mm3. I guess this add to mass scaling to the model. I am aware that I cannot use kg/mm3 as a density unit if I need to have consistency with my length being in mm, force in N and Properties of material in MPa. Initially I tried running double precision but it gave me error while running simulation for eulerian analysis so I had to avoid it. But may be in future with higher modelling I may need to use double precision.

As my model require very fine mesh at the tip of needle, I have the stable time increment of 1.01e-9 which is quite small which add up to high computational time.
I am trying to use mass scaling of those critical element which has time increment below 1.01e-9.

Would you think that will make the model to run the simulation with less computational time and without any error and complete the analysis?

One more thing I have the needle meshed in hexahedral element with 2 layers of mesh. Would it make any good if I make one layer of meshing throughout the needle instead of 2 layers and it will increase mesh size. Or tetra element be any good for similar problem?

Thanks.

 

[Dave442]

Hi,

Like I said previously, if your model doesn't complete with consistent units there is a problem somewhere. You can't just scale the mass by three orders of magnitude without a justification beyond "it helps the analysis complete". Would you scale the elastic modulus or applied load by three orders of magnitude? Probably not. Mass- and time-scaling are used to increase the size of the stable time increment in quasi-static explicit analyses where the velocity is low and the kinetic energy is very small relative to the internal energy. You typically monitor the ratio of internal/kinetic energy during the analysis to ensure that it remains quasi-static throughout.

If you are using a fine mesh you should probably be using double precision. Just because your analysis fails to complete when you specify double precision does not mean you should avoid it. Check the .sta file for a warning regarding solver precision. You should see it after the first increment results. Can you post a picture of your mesh?

Dave

 

[IRstuff]

Hypothetically, the OP is not scaling density at all --> 7.8e-6 kg/mm^3 = 7.8e-9 tonne/mm^3 The densities are numerically equivalent.

TTFN
I can do absolutely anything. I'm an expert!
faq731-376 forum1529

 

[mgj2015]

Hello IRstuff,

I agree hypothetically there is no difference between density at all --> 7.8e-6 kg/mm^3 = 7.8e-9 tonne/mm^3.

Question is Can I use the kg/mm3 instead of tonne/mm3 to define the density when I have model in millimetres (mm). Would that make any difference in output as the metric system would be not consistent. force will be still in N and model in mm.

Dave442 would you agree to this. I don't know what is the issue when I keep the density in kg/mm3 instead of tonne/mm3 and rest in MPa, mm the model tends to run smoothly and completed at very less CPU time.

 

[ThomasH]

Hi

The densities are numerically eqvivalent. But, does ABAQUS have a "built-in" unit system or does it fall on the user to encure that. Like I said, I don't work with ABAQUS but I do work with Nastran and there is no unit system. It is the user's responsibility to ensure consistency. What units have you used for the other parameters?

If you scale a mass 1000 times, you might get a solution but does the solution simulate the physics of the problem or is it something else. Mass-scaling is a trick that should be used with care. If the inertia forces are of interest, they will be wrong.

Thomas

 

[mgj2015]

Hello Thomas,

No abaqus don't have unit system. Its user responsibility to ensure consistency.

I have the model in mm, modulus and yield in MPa and density in kg/mm3. I initially tried with tonne/mm3 but that resulted in element failure in the tip of needle. So I changed the density with kg/mm3 and the model run smoothly for the same with no element failure.


My model is needle displacement into the rubber based eulerian analysis. The needle travel through the rubber material up to 10mm. I am trying to find the resultant force for given 10mm displacement.

I HAVE ATTACHED THE NEEDLE MESH IMAGE OVER HERE

 

[Dave442]

Hi,

7.8e-6 kg/mm^3 and 7.8e-6 kg/mm^3 may be numerically equivalent densities but you need to specify the one that is consistent with your adopted mass, length and time scale. In the case that you have specified your geometry in mm, forces in N and time in s, you must specify density in tonne/mm3.

The mesh at the point of your needle does not look great - the elements are long, thin and skewed. It is these elements that deform and become distorted when you use the correct density. When you scale the density I guess these elements don't see as much deformation and the analysis completes. But you have no justification for doing this?

Also, if your testing is dynamic or your material model for the rubber is rate-dependent you will be messing with all of the inertial terms by scaling the density.

Dave

 

[mgj2015]

Hi Dave,

I have meshed the same needle with finer mesh then what are u looking at long and skewed. I had meshed with 3 element in a row, 4 elements in the same row and now u can see 2 elements in the same needle tip row. The mesh at needle tip play only a part of role in distortion, where as stiffness play the main role.

So you think if I use kg/mm3 then I am scaling the model to 1000 times w.r.t to stiffness. I don't know if hypothetically kg/mm3 is equal to tonne/mm3, y would the result will be different and simulation has complete different approach towards running of simulation.

Regards,
MGJ

 

[ThomasH]

Hi

So density should be tonnes/mm3 and not kg/mm3. Now you are scaling the mass 1000 times, not the stiffness. The typical reason for mass scaling is to get a more reasonable timestep.

In your case I don't know exactly what is happening but you introduce an error to get a result. The problem is that the result may be erroneous due to the introduced error.

Why not try with a smaller model and see if you can figure out why it fails?

Thomas

 

[Dave442]

Hi,

If you're trying to correlate your FEA force-displacement data to test data could you neglect the deformation of the needle and model it as a rigid part? That way you avoid excessive element distortion (as there is no needle deformation) and you no longer need to specify material properties for the needle so your stable time increment is not scaled by the very fine elements at its tip. If your needle is significantly stiffer than your rubber material your results might be OK? worth a try.

As you are running explicit I assume you are using reduced-integration elements and as you have only one layer of brick elements through the thickness of the needle tip at it is unlikely that you are currently capturing bending effects anyway.

Dave