Workflow to streamline repeated model change/query/change/query 1

[Sparweb]

Hi
I'm still very new to FEMAP so hopefully there's a simple or obvious solution.
I have set myself up for a long slow workflow on an model of dozens on interlaced beams where I must find the stiffness in all 6 DOF at 16 specific points within the model.
My current workflow is to apply one unit load at one point in one direction, Analyze, Query the displacement at that point in the corresponding DOF, then delete that load and start again, with the next unit load in the next DOF.
Each change/query/analysis takes about 4 minutes per DOF, so 6 DOF at each point takes 24 minutes to complete, therefore the whole procedure will take all day.

Is there a way to streamline this process? I've considered applying all of the unit loads in separate load sets, then setting up analysis sets for each load set... there would be about 96 of them. This could churn away while I did something else, and then upon completion I could find some way to "scroll" through the result sets while extracting data. This might save a few hours if I knew it would work. The only query I know of if from the Info pull-down menu. Can I select all of the result sets before displaying the translations and rotations?

STF

 

[RCatania]

You can set up your 96 load sets rather easily (or a custom API can be written to further automate), then use the “MultiSet” button in the Analysis Set Manager to create 96 Subcases with a single command. In addition, if you are not changing your constraints, then NX Nastran only has to invert the stiffness matrix a single time, then apply each load set, which should save a reasonable amount of time when solving.
You can then use “List, Output, Results to Data Table”, select any number of Output Vectors in any number of Output Sets to query your data. It would also be easy to send the data to Excel.

If you are interested, we have an Introduction to FEMAP Training Class that provides a great overview of FEMAP functionality.

http://training.plm.automation.siem...filterseats=&seatscond=gte&sort=software&pg=1

Additionally, please refer future questions to the regularly monitored FEMAP User Community. You can navigate to the site from within FEMAP by using "Help" \ FEMAP User Community.

https://community.plm.automation.si...tion-Femap-Forum/bd-p/Simcenter_3DFemap_forum

 

[rb1957]

Hi Steve,

I get what you're doing, but remember to include the secondary effects at the other freedoms; it's not just apply a load in one freedom, get the deflection, determine the stiffness. It'll be a 96x96 stiffness matrix.

Is it possible to run the two models together ? (I figure you're extracting the stiffness of one model to use in another.)

Is it possible to use NASTRAN, to get a .kaax (I think) equivalent stiffness ?

another day in paradise, or is paradise one day closer ?

 

[Sparweb]

Hi RCantania,
I just took the Intro class and I'm jumping in with both feet, here.

You can set up your 96 load sets rather easily (or a custom API can be written to further automate)

That still sounds like separately defining all 96. Copying load sets still must be done one at a time, just as fast if not slower than creating new sets one at a time.
Looking at the multiset analysis I think I see how that avenue works, but I need to define all the loads sets first.

Looking at the structure, I am narrowing down the problem by symmetry, but that may only cut it by half.

STF

 

[Sparweb]

I also just found the Data Table. That should help. Previously I was picking the node after each run.

STF

 

[RCatania]

Here is a video I made that may be a good method for you. Using Excel, and then CSV, you can create "Table Output" in FEMAP then create load from that Table Output.

https://community.plm.automation.si...136/video-id/pvZXFhYTE6EYQn2GVOIgZDcjDKkg_d62

Your question is probably a great candidate for an API to help automate the creation of your load sets. If you could use pictures to describe your process I could write a script that should speed things up for you.

In addition, here is a throw-away google e-mail I've made if you want to send me a sample of your model or other info.
burnengtips@gmail.com

 

[Sparweb]

Hello again,
I watched the video - appears to import loads quite efficiently, thank you!
I do know the nodes in question, so that much is helpful. Can these loads be imported to separate sets, or just one load set?
If they are all in one load set then the analysis would apply all loads simultaneously, rather than individually.

Still, plenty of cases where this will help a lot - first thought is to distribute a pressure load to multiple loads, or as a means of growing the loads on a node in increments by re-importing the loads from the spreadsheet. If the load case is complex this would go a lot faster.

STF

 

[RCatania]

With the method described in the video, that would require you to repeat the process 16 times, if you wanted to create new load sets. 16 is better than 96, but if you are creating loads that can be incremented, such that load set#2 = 2* loadset#1.. etc... you could use the Data Surface Editor (Tools \ Data Surface Editor, or Toolbar Icon)

I will also attempt to write an API for you based on the import method.

 

[TG_eng]

SparWeb

What type of load are you creating? Force, moment, displacement, etc...?

Are you looking to create multiple sets of just one type or a combination?

 

[Sparweb]

RB and TG,
I think I can answer both your questions together.

An installation of several identical monuments on the cabin floor is being modeled in FEMAP. Model 1 of a monument is used to demonstrate its structural strength, Model 2 of the floor is to discover the displacement of the floor given the reaction loads from the monument attached to it. Unfortunately, this project has had many many hands in it, so the floor and monument were modeled separately. I'm the third to have a hand in the modeling, and I'd be at a loss to unite them now.

I've been able to simplify my repetitive problem, by treating it as a "sensitivity analysis" rather than a "compendium of nodal data". Looking at the 4 monument locations, it was fairly easy to select the stiffest and the softest two locations (problem divided in half). Then looking at the attachment fasteners for each monument, the ones closer to the fixed ends of the floor beams have much less deflection per unit load, so I reduced the problem yet again, by half. I was able to get all of the upper and lower bounds done this morning, just by having a better strategy. I also had time to sample other locations that I wasn't testing in detail, just to make sure my assumptions were correct.

The sensitivity analysis can now move forward. The stiffness of the aircraft floor is being entered into the model of the monument as DOF spring elements. This will provide a very different set of reaction loads at the fasteners attaching the monument to the floor, compared to the fixed restraints it had before. Especially the secondary reaction loads. Total translation is much higher on the softer supports. As expected.

Is it possible to use NASTRAN, to get a .kaax (I think) equivalent stiffness ?

Don't know what you're talking about there. Still wet behind the ears. Sounds interesting though. This is NX NASTRAN.

This won't be the last time I do something like this, so I look forward to being better prepared next time. Knowing where the sand traps are is half the battle.

STF

 

[Sparweb]

I will also attempt to write an API for you based on the import method.

Wow! Very generous of you. I hope you see my recent posting about finishing early by redefining the problem!
While I know I will appreciate the use of API's in the future, I still struggle with the basics like creating geometry and meshing even the simplest things. I gotta learn to walk before I run.

PS Sharing models outside the company is strongly frowned upon. I'm surprised how often I get asked this. Your help is appreciated!

STF

 

[rb1957]

Hi Steve,

So you want to measure the impact of 16 monuments on the floor/fuselage structure ...
I get where you're going ... forget the sand traps, keep an eye out for the crocs ! I think one (or several) are eyeing you up now !?

If the monuments are loading frames pretty directly then are the monuments talking to one another ? Maybe it's enough to sum adjacent monuments and call it a day ?

If the monuments are loading the seat tracks, now you've a different problem (to get the frame reactions) with seat tracks being continuous beams over several frames; but that's an easy enough analysis (hand calc or FE).

But this could be where you are ? the monuments are not simple structures (ie near enough similar reaction stiffness so they can be solved in isolation then apply the loads to the seat tracks) but you're looking at these monuments as floating on the seat tracks. I think the easiest way to solve this is to model the seat track(s) and their frame supports (equally stiff) and simplify the monuments to an RBE2 (or maybe a very stiff frame). I suspect that the result should be much the same as assuming equally stiff supports.

clear as mud ?

another day in paradise, or is paradise one day closer ?

 

[Sparweb]

Haha, thanks for muddying the waters.
Those ideas could have been considered at the beginning (before I got involved) and I can't relate to you now how the choice was made to build the separate models the way they are. They work just fine, independently... it's the relationship I'm building now. Got that under control, too, now that I have the stiffness values in a spreadsheet. The DOF spring elements at the floor reaction points are now in the monument model. Makes a dramatic difference after previously using fixed reactions (obviously).

Putting the monument reaction loads into the floor model... there's an interesting thought. Not what I was asked to do, but not as time consuming as the job I was envisioning in my OP. It would take a few iterations, going back and forth between monument model to get the reactions, the floor to apply them at get the deflections, then going back to the monument to update the DOF springs... also a whole day's work but more fun to watch things evolve.
But it sounds more like "model validation" than "sensitivity comparison" so until a big red flag gets raised I will not turn this into a science project.

STF

 

[Sparweb]

RCatania,
I have posted a follow-up question in the FEMAP user's forum as you suggested. There's a screen shot of the floor model I'm working with.
It's a very esoteric question, however. It has more to do with the way FEMAP creates deformed views, and what could go wrong...

https://community.plm.automation.si...Deformations/m-p/441587/highlight/false#M5800

STF