I am working on a complete ship model in FEMAP, where I encounter an issue I could use some advice for. I apply hydrostatic pressure loads on the surfaces of the hull of my model, and similar pressure loads to the cargo hold (the ship is a TSHD vessel) and some other tanks. When I want to export the analysis model containing 6 load cases with each these kinds of loads, it takes more than an hour to create the *.dat file. I suspect this is because of the internal translation step of loads on surfaces to loads on associated elements, but I cannot imagine why this would take so long...
In the past I have added my loads directly to elements, which made the process of exporting an analysis model very fast, but I decided to change to the "loads on surface" approach, since I don't want to reapply the loads every time I am refining locally a surface mesh panel.
My model contains about 27K surfaces, with an 80K elements, of which 8K are on the hull of the ship. By way of example I added to the attachments a model of a hull (the red part is 7400 elements, loaded with hydrostatic pressure, the green part is there to accumulate to 80K elements on 27K surfaces). This model takes on my HP Z440 Workstation (Intel(R) Xeon(R) CPU E5-1650 v3 @ 3.50GHz, 3501 Mhz, 6 Core(s), 12 Logical Processor(s), 16GB RAM) about 4 minutes to export. As you can imagine, this will add up to 3 groups times 6 loadcases times 4 minutes (~72 minutes!) for a full model.
Does someone have any idea how to speed up this process? Or perhaps a general suggestion what method is more efficient to take in FEMAP anyway?
Cor van Dijk
TL;DR: What is the reason that applying loads on surfaces makes the process of exporting an analysis model to a .dat file so slow?
Solved! Go to Solution.
First at all you FEMAP model is done using an older version of FEMAP, I suggest to update URGENTLY!. I remember reporting to FEMAP developers a similar problem running FEMAP V11.1 of spending more than 4 hours witting the *.dat file, BUT using a new version 11.2 the problem was written in 5 seconds!!. Then is good to share this type of models with FEMAP developers, this way they can investigate an improve FEMAP, OK?.
Open Model Opening model file from Femap version 11.10
Second, you have some inconsistency in your FEMAP model regarding mesh density & element thickness: if I plot elements by thickness you see the result, the Shell CQUAD4 element size is 1 mm when the thickness is 10 mm!!, this is not reasonable.
Also I note you have ONE isolated surface per element, then more than 27000 surfaces for 81000 elements!!. In my opinion this is the reason of the lack of performance, you have many, many isolated surfaces, not stitched, then FEMAP takes a lot of time to expand & compress loads??. Let's investigate if this is the reason.
1.- I simply used command GEOMETRY > SOLID > STITCH and selected ALL surfaces of your model. The key here is to use a correct tolerance (in general I use 1e-4 for models in mm, but for a REAL HULL of say 50 meters this can be 1e-3, simply is a question of try!!) and in this case to set OFF the cleanUP mergeable curves, this way you can save the original surfaces edges to apply pressure. The YELLOW line shows you that all the surfaces are correctly stitched, and now only ONE sheet solid body exist in your FEMAP model!!.
2.- Next I associate the new created Sheet solid with the mesh using command MODIFY > ASSOCIATIVITY > AUTOMATIC, selecting all the elements with the new sheet body.
Automatic Associativity 81154 Element(s) Selected... 1 Solid(s) Selected... Attaching to Solid 1... 27787 Nodes associated with Point(s). 36432 Nodes associated with Curve(s). 18202 Nodes associated with Surface(s). 0 Nodes associated with Solid(s). No geometry associated with 0 Nodes. 81154 Elements associated with Geometry. No Geometry associated with 0 Elements.
3.- I revise the correct application of pressure loads.
4.- And finally if I create a new analysis study and perform PREVIEW ANALYSIS I note it takes now around ONE MINUTE to write the *.dat file (I performed the same task in your original model and the time cost was 4 minutes!!).
Then, here you are my findings, if you use the above workflow you will improve the performance of your model. Also, I always suggest to base pressure loads in geometry, not mesh, this way you can control better the consistence in SHELL NORMALS, another common error found in users many times, OK?.
Thank you for your swift reply. I will definately ask for an update of my FEMAP, I am looking forward to spending less time in creating the analysis model file :-)
Regarding the steps you propose, I work indeed with 1 solid per surface. The reason I do this is that I haven't found a way to update surface normals separately, when they are part of a single solid. But I will give your suggestion a try; I am looking after all for a good way to use FEMAP in combination with large models that need frequent modications. The element thickness issue is my bad, I normally work with mm models, and now I quickly made a m model but loaded the properties of my mm model...
Once again, thanks for the help, and I will keep you posted regarding results with an updated FEMAP version.
Cor van Dijk
Precisely an important benefit of the use of GEOMETRY > SOLID > STITCH command in FEMAP is just this: if you stitch a group of surfaces, each one having different normals, then the resulting sheet solid body will have a common surface normal, either all OUT or all IN. This is very important, because later when you mesh the sheet solid surfaces then all Shell elements will have correct normal consistence, OK?.
The above STITCH command is valid for continuous surfaces, without any stiffener o "T-Junctions", for instance your HULL geometry. But if you want to include stiffeners or any other T-JUNCTION geometry then you should use command "GEOMETRY > SURFACE > Non-ManifoldAdd", but here the surfaces will be added to the nonmanifold sheet body preserving its original orientation, (ie, surface normal), then you should run with caution to make sure that all surfaces will be oriented correctly because later (once created the nonmanifold) is not possible to reorient any surface individually, the command MODIFY > UPDATE OTHER > SURFACE NORMAL do not run with nonmanifoldAdd geometry, OK?.
They way I run is to use the STITCH command will all non-branching surfaces, where available, and later combine all stitched and non-stitched bodies everything using NonManifoldAdd command, this is the better workflow.
Please note that current version of FEMAP V11.2 allow to use with NonManifold sheet bodies geometry most of the commands under GEOMETRY > SOLID like SLICE, etc.., in the old versions of FEMAP it was not possible at all.