Import Nastran .pch file that contains DMIG information (stiffness matrix?)?

[hootrpootr]

First of all, I’d like to apologize for any misleading information or confusion I may cause, as this is a topic I’m very unfamiliar with.

Basically, a customer provided me with a set of files with which to create and run a model using Patran with Nastran.

All of the files except one make sense: patran database file, load cases bdf, loads bdf, etc. The one file that I know nothing about is a .pch file that contains lines of code referring to “dmig kaax”, “dmig paax”, and referencing various nodes in the model. I know that the nodes are all interface points that connect one major structural assembly to another. And based on a google search, I’m under the impression this .pch file has something to do with the stiffness matrices at the nodes.

I hope this is enough info to go off of, but is a .pch file something that is exported out of a database, or something I can import into one? If it’s the latter, how could I accomplish this?
Thanks!

 

[dmapguru]

That .pch file is one of the output files from an MSC Nastran run. I am inferring it emanates from an external superelement creation run because the names of the DMIGs (KAAX and PAX) are standard names that the EXTSEOUT case control command will affect to the DMIGs.

OK, so you can't do a great deal with these data in Patran.

What your customer has provided to you is a reduced component probably created as an external superelement. As you rightly surmised, the KAAX matrix is the stiffness of the reduced component as seen at the boundary connection points. As long as you have the GRID points that go with the DMIG entries, you have a complete data set for the reduced component. Just keep the DMIGs to one side and prepare the remainder of your model, making sure you keep the GRID points connected to the DMIGs in the same location with the same numbers. The PAX matrix is a load matrix, presumably some loads were defined on the interior points of the reduced component (you can't see these points, but you can apply the loads on them via the boundary PAX data - see the cautionary note about loads below).

To use the DMIGs, you will need to "activate" them when you run the job. Either copy/paste the DMIGs into your input file along with the other model data, or you could use an include statement to include the file containing the DMIGs inline with the other bulk data in the input file. In the case control, above the first SUBCASE command, add the lines

K2GG=KAAX
P2G=PAX

This will activate the DMIGs with these names; the KAAX boundary matrix data will be added to the total stiffness and the PAX data to the loads prior to solution.

Now, careful with the loads. If PAX contains one column (i.e. one load case), then it will be added to the first load case (SUBCASE) when you run the model with the DMIG data attached. If PAX contains more than one column, the load cases in PAX will be added to the SUBCASEs in the analysis in sequential order (column 1 of PAX to the first SUBCASE, column 2 of PAX to the second SUBCASE and so on). There is no way to apply column 2 of PAX to the first SUBCASE in the job. A workaround is to define a dummy load case with no load or a dummy load and ignore the results.

DG