Ansys Designmodeler question? 2

[engltayl]

I am just starting out at learning DM. I have modelled a tube with some cutouts as a mid-surface shell structure. I want to send this model into ansys classic for some non-linear dynamic work. There are a few things i cant get to grips with

1. I cant seem to be able to export a named selection into ansys so that it comes up in ansys as a component.

2. Say i want to apply a pressure to a specific area of a face, can i somehow draw this area in DM, give this a named selection, so that when i export to ansys classic it is easy to select the pressure location

3. Up to now ive just been exporting the geometry out of the DM via a *.ans file. I would really like to use simulation, mesh the model, add loads/constraints, and then import into ansys for processing. The problem i have is that simulation only seems to mesh in shell-181 elements and not shell-93 which is what i want. There is an option for higher order elements in the mesh options but it seems to be greyed out. Is there a way to force a specific element type?

Sorry for going on, but i struggling.

Thanks for any help!

 

[cbrn]

Hi,
1- I don't know if the named selections made in DM are transfered to Classical; probably not, you'd better define them when you are in Simulation. From Simulation to Classical, the named selections ARE transfered, I know it for sure because I use this constantly. Surface components will be converted into nodes components, so if you make a named selection on an unmeshed surface, this won't produce any result.
2- Once again, I don't know if DM allows you to cut a region from an area (it should, at least as intersection of two areas, but I'm not sure since I don't have the license for DM), but if so, then in Simulation you will see two separate areas and yes you can select the loaded one and insert it into a named selection, thus returning to Point 1.
If you still have troubles like this, try and see if DM has an option to save Parasolid or IGES geometry; then you could read it directly into Classical.
3- From the Simulation manual, it appears that the only shell elem type supported in WB is SHELL181 (1st order elem). There is no simple way to get rid of this limitation. You can override WB mesher by adding your own APDL in a "Commands" object, thus defining elem type / real constants just like you would in a Classical script, but the mesher invoked by commands such as AMESH will be the one operating in Classical, thus loosing all the "smartness" of the WB one.
At this point, the best thing you can do is to change elem type inside Classical AFTER having your model meshed inside Simulation. The sequence of commands invoked will be EMODIF and EMID (change to 2nd-order elem, then add midside nodes) - see the ANSYS manual for more details: section 9.2, chapters 9.2.6, 9.2.7.

Hope this helps...

Regards

 

[doatis]

Hi,

1 - You are correct, named selections in DM do not translate into geometry named components in ANSYS Classic. In Simulation, Named Selections are carried across as either nodal or element components. Named selections from DM can be brought into Simulation, and if you use the Simulation mesher you can then access the FEM components

2 - What you want to do is an 'imprint face'. Select the area you want to divide into a pressurized/non-pressurized feature. Then sketch your pressurized area on it. Next, make sure the body is unfrozen (you can't imprint on a frozen body). Then extrude, use your sketch as the base object, set the operation to imprint face, and generate. This will trim the surface. You can't create a named component that carries over in DM (see my response to 1), but same rules apply for using the Simulation mesher

3 - You are correct, you currently can't set a shell element to be a low order element. However, you can easily strip out the midside nodes and switch the element type in classic (use emid command). Just to let you know, in v11 (due out later this year), you are able to specify whether or not to keep the midside nodes.

If you really want to get fancy, you can insert a command snippet on the part to modify the elements. Right click on the body, insert, commands. In the command snippet, use the emid to remove the nodes, then redefine the element type. However, this will cause some issues with reading in the results after the solve (since what ANSYS generated isn't the same as what's coming back).

Just a sidenote, unless you're limited by computing resources or something else, you should stick with the midside nodes. Also, unless you're doing some exotic post processing, the Simulation post processor is as good as, if not better, than the Classic /post1

Good luck!

 

[engltayl]

Thankd for your help guys! Think i may have stumbled across the imprint faces feature today. but when i imported the anf file into ansys classic. I got an area over another area, hence i got elements over elements when i meshed.

Also, the analysis im doing requires placing a varing load with time and non-linear material data. can this be done somehow in ansys workbench. From what i read it cant, hence why im exporting my geometry to workbench.

Also (sorry), when i export a meshed simulation from workbench simulation using the 'write ansys input file' i get the meshed geometry in ansys classic but i dont get any lines, areas or keypoints etcs. is there a way to force this?

thanks again...........

 

[cbrn]

Hi,
there is no direct way to have WB export the solid part of the model into Classical: WB will only export the FE part. One note: you can avoid manually creating the ".inp" file: you can call the Classical interface from within WB.
You could try (I never did, so it may not work...) to add a Commands snippet including the following APDL commands:
/PREP7
CDOPT,iges
CDWRITE,solid,<filename>,<extension>,,<iges filename>,<extension>

Non-linear material data can be defined in WB. WB also includes the capability to handle transients, and to define different loads at every loadstep (well, better said: define loads that vary between the loadsteps), though I don't know if it is possible to define them by expression instead of discrete values. Anyway, if you know how to operate with table-defined loads, you can do anything you want with APDL.

 

[doatis]

Here are the two export options you have:

1 - Export the solid geometry from DM without a mesh and do the rest of your preprocessing (material definition, meshing, loading) and post processing in ANSYS Classic

2 - Export the meshed model from Simulation with all the loads, solve, and post process in ANSYS Classic

I have a gut feeling that the cdwrite trick won't work, for this reason: Simulation has no geometry attached to it. The only thing it does is mesh/load/solve/post process the model. If you look at the Solution Information while the solve is going, you'll see that at no point does solid geometry come into play. The command snippet will occur after the nodes/elements have been passed, so you won't get any geometry out of it.

As for loads defined as expressions, that is a capability that I have seen in releases of v11.

I also agree...if you know APDL, you can do anything in WB (not just tabular loading)

 

[engltayl]

Thanks for your help again...

sorry another question...

when i mesh a surfaced model in simulation and export to ansys via an input file i get MESH200 elements. Can i not mesh in shell elements?

cheers

 

[doatis]

The reason you have mesh200's is because you haven't requested any structural results. If you request a structural result (i.e. total deformation, stress, strain), it will be meshed with structural shell elements. If you request a thermal result (assuming you have thermal loads), it will be meshed with shell elements.

Workbench will use mesh200's as long as there is a question mark in the Simulation tree. You should see a question mark next to Environment and Solution, since Workbench doesn't know what type of analysis you're doing (structural/thermal/emag/etc.), so it doesn't know what DOFs to solve for...meaning it doesn't know what elements to use.

 

[engltayl]

How stupid am i! thanks for the help...much appreciate it!

 

[cbrn]

Hi,

just to avoid that you spend time trying an unuseful thing: this morning, just for curiosity, I tried and add a Commands "cdwrite" to the Part object in Simulation, and I used the "Comb" option. Anyway, this produced no solid result, as expected...

It's not totally true that Simulation knows nothing about solid geometry (if so, it wouldn't be able to mesh anything...): simply, it stores and handles it in a topological fashion which is totally incompatible with the method used by Ansys Classical.

Regards