mass scaling

[andrearrd]

hello.
I am trying to model a stent in Abaqus. Basically i am running tests wher i apply an internal pressure so the stent (cykindrical shape) expands radially until it deforms plastically. I apply this pressure load in a dynamic time step. I then have another time step where the load is removed, and the stent, since deformed plastically, should stop exp-anding and remain in the same shape (roughly speaking). The problem i have is that it keeps expanding during teh second timestep even when the load is removed. i suspect this is from the fat that im using substantial mass scaling in order to increase the simulation. is there any other way to increase the speed without having to use mass scaling.

thanks very much
andy

 

[corus]

Try and have a uniform mesh and avoid small elements as the time step in explicit will depend on the smallest element. You could make your mesh a lot coarser in general to increase the speed of the analysis but then you lose a certain amount of accuracy.

corus

 

[nagi]

Why aren't you doing an implicit analysis?

 

[Drej]

As nagi says, why the need to perform an explicit analysis? It doesn't sound like your problem is dominated by inertia effects (except now that you're mass scaling of course), so it would appear sensible to carry out an implicit analysis. An implicit analysis would be especially appropriate if you're interested in residual stresses after the load is removed (although you could do an explicit-to-implicit results transfer for this if necessary).

-- drej --

 

[corus]

In general an explicit analysis is more stable in complex contact problems than an implicit analysis. Residual stresses are still produced by an explicit analysis.

corus

 

[Drej]

Of course, residual stresses can be modelled using explicit methods, but because of the nature of the explicit algorithm it usually leads to economically unfeasible analysis times, hence why ABAQUS provides a facility to perform an explicit to implicit transfer for this type of analysis. It is correct to say that, generally, the explicit contact algorithm is more stable. The key issue here though, is: why is it necessary to obtain an explicit solution for what appears to be a fairly simple and straightforward problem? Is the contact so complex and the time span of the load short enough to justify an explicit solution? It may require some more details of the problem, but I would almost certainly be happy in justifying a implicit approach here.

Only imho, of course.

 

[nagi]

I agree with Drej that it all depends on the specifics of the model which we don't have that much information about.

For such a slow speed process implicit analysis (with the right contact settings) will usually work. In many cases, such as this one where mass scaling is significantly affecting the solution, getting the implicit analysis to work is worth the effort.

Alternatively, you may stick with explicit analysis but with less mass scaling and accept the resulting smaller time step size.

Nagi

 

[andrearrd]

thank you everybody for ur help. will try using implicit now

 

[andrearrd]

ok i am using explict now and it is much quicker. however i have one question, whihc is prob quite stupid but i havent used abaqus that much. i can get the expanison to work, but then io remove the load by having another time step with the load inactive. this is too see if my stent remains deformed plastically. i get an error saying too many increments have been attempted. how do i get rid of this? thank you in advance

 

[nagi]

I guess you mean that you are now using implicit analysis? In that case, you should reduce the load gradually instead of just removing it at once.

 

[corus]

The load will be reduced gradually as the time step is reduced for each increment and so the problem won't lie there. I'd check to see why you are getting too many increments. Usually it's due to the contact not being resolved. See if you're getting chattering where for each successive iteration you get a few closures followed by the same number of openings. You may have to review your contact surfaces or stabilize the contact procedure to inprove convergence.

corus

 

[andrearrd]

thanks. i will modify the load to increasing lineraly , then staying at a constant value, and then decreasing linerly back down to 0. i think the only way is though a subroutine, whcih i have written in fortran and compiled but when i submit the job, nothign seems to happen.

 

[corus]

There is no need to write a subroutine to increase the load. The load is automatically ramped through the time step. If you don't apply a load in the last step then it is ramped down to zero from the previous value. Check the *step in the manual to make sure.

corus