In the linear statics solution sequence (101), is there a way to get the results of each subcase to feed into the following subcase, similar to the way it automatically happens in the non-linear statics solution sequences (specifically 106)?

Are you able to use SOL 400? DMAP is a solution, do you have the time to QA your process?

Is there a reason you don't want to use SOL106? If you don't have any nonlinearities, then just set PARAM,LGDISP,-1 (the default) to use small displacement theory, and give the NLPARM a single increment (or maybe just a few increments). If it is truly 'linear' then it should converge rather quickly.

I read up on Sol 400, and it looks like it would ​have worked, but unfortunately we don't have it as part of our license.  I am beginning to think it will have to be via DMAP.  By QA, are you referring to running some check cases against the DMAP altered solution?

 

Also, a little more background.  I am doing a gravity release analysis similar to what was done on NASA's Chandra observatory (I can mention that much since there was a paper presented on this analysis back in the 1995-97 time frame that is in the public domain).  That was long enough ago that they were using Solution 66.  The intent of the analysis is to see what the level of residual strain exists in the payload after going through its assembly sequence and then placed in a zero G environment analytically.  Their approach consisted of creating two subcases for each assembly step; the first is to have both unconnected subsystems kinematically fixed via base point SPCs on one subsystem and lift point SPCs on the second subsystem in a one G environment, and the second step is to join the appropriate subsystems' connection DOFs with MPCs and remove the one G environment.  I am emulating that process using solution 106.  After looking at the description of what the authors  did, it seems clear that while the overall process is non-linear, the two individual subcases are both linear; they are simply using the non-linear solution because it automatically feeds each subcase results into the next subcase.  My problem is that the way the current model's materials and properties are set up, the 106 solution sequence is giving me fatal errors because it apparently requires the 12 I/t^3 field on PSHELLs to be unity or blank (several PSHELLs have a different value to provide greater bending stiffness resulting from the use of layered composites as opposed to a homogeneous shell) and it didn't like (as in FATAL error) the materials specified - apparently you are restricted to a MAT1 and MATS1 combination.  In my latest attempt, I specified ANALYSIS = STATICS in each of the subcases hoping to force it to treat each individual subcase as linear, but that didn't work - I still got the same fatal errors.  This was quite long winded, but I felt like it might direct everybody's recommendation in a more specific direction,

To respond to Don Graff, I would very much like to use 106, since it does automatically feed the results from each subcase into the following subcase. I will try that PARAM to see if it will force it to go linear and bypass the errors produced that I described in my (very long) earlier response.

Yes, by QA, have a known answer, maybe more than one, to verify the results are what you expect. Plausible but wrong answers seem to be easier to 'calculate' more than ever.

 

I have seen DMAP that takes preloading in one subcase and transfers the DIFFK and the displaced shape to another subcase. Part of this became the GRAVSET and RFORSET options via PARAMs in V2019. This might be a good start for added DMAP work.

 

 

If we need to address the FATAL errors as a support case, let me know... it would be best to stay within the standard process using SOL106 if possible.

Will do. I understanding from this comment that resolving fatal errors needs to be handled via a different support service path.

Unfortunately the LGDISP parameter had no effect. I believe I will get a compiler listing and start working a DMAP path...

 

Can you cut and paste the FATAL errors (and any corresponding warnings) here? Or when contacting MSC for support, ask for me (Don Graff) since I am already 'thinking' about this!

The first fatal error:

 

 *** USER FATAL MESSAGE 2083 (TA1NLE)

    FOR NONLINEAR MATERIAL PROPERTIES REFERENCED ON THE PSHELL ENTRY, 12I/T3 FIELD MUST BE 1.0 (OR BLANK).

 

The second fatal error, after converting all the offending PSHELL 12 I/t^3 fields to unity:

 

 *** USER FATAL MESSAGE 2083 (TA1NLE)

    FOR NONLINEAR MATERIAL PROPERTIES REFERENCED ON THE PSHELL ENTRY,

    MID4 MUST BE BLANK AND MID1 AND MID2 MUST REFERENCE THE SAME MAT1/MATS1 ENTRY COMBINATION.