FEA Chassis Analysis - Ansys Workbench

[eklipse]

I have some questions for frequent users of Ansys Workbench. I typically use Ansys Classic for my analyses, however, I am switching over to Ansys Workbench and am having difficulties achieving the same results.

I've modeled my frame in Solidworks with suspension and various mounting brackets and exported the assembly as an IGES file (Manifold Solid B-Rep Object, Type 186). The exported IGES file contains only a 3D line sketch of the frame and the mounting brackets as Solids floating in their relative places.

I have imported the file into an Ansys Workbench geometry file where it generated Line Bodies for the 3D line sketch and the Solids Bodies for the mounting brackets. I have assigned appropriate cross section attributes to each line-body in the Geometry File and have meshed the elements in the Simulation File.

This is where I have problems.
1) When I apply loads and constraints, it appears that all the individual beams are floating in space and will deform independently from the other beam members, as if nothing was connected. I have seen other beam analyses where the frame was merged into one single part, however I get an error when I try to solve the Solution that says "An internal solution magnitude limit was exceeded. Please check your Environment for inappropriate load values or insufficient supports. Also check that your mesh has more than 1 element in at least 2 directions if solid brick elements are present...". I will try to verify that my model is correct, but I can't seem to avoid getting this error.

2) Connections/Contacts. I cannot make any contacts or joint connections between the mounting brackets and the line-body beam elements. The Connection tool won't let me select lines or line bodies. Any suggestions?

3) Driver weight. I wanted to add a Point Mass to simulate the inertial forces of the driver sitting inside the vehicle, however, the Point Mass Feature seems to only apply to faces, whereas I have mentioned before, I only have line-bodies for the frame. Any ideas on how I can apply these loads? I suppose I could model a seat as a surface but that leads me back to Problem #2 where I can't seem to make any connections between line-bodies and anything else.

Any suggestions would be much appreciated.

Thanks,

Adam

[FormulaJuan]

My experience with ansys is pretty elementary, but i'll try and relate my knowledge to help you..


For beam type structures (space frame), we always use Ansys "classic". In ansys we define the analysis to a beam type analysis. From what i understand, if you import something as an iges into workbench, it will analyze it as a solid. This is much more time consuming and less accurate than the traditional beam type algorithms within ansys.

I would just input all the keypoints into ansys, define your lines, define the mesh, yadda yadda yadda, then analyze that. Just make sure your material props and whatnot are the ones you should be using.

[FormulaJuan]

For the record, thats how we analyze our frame.

[frenzy]

can anybody give me a clue how I could "easily" import keypoints from a solidworks 3d-sketch into ansys?
it's a pain in the a** to type them in manually ..

[DonMolina]

You know, you could use COSMOSWorks.

Works just great, and integration with Solidworks enables you to chage anything you wan on the fly so that you can do a lot of studies without having to go back and forth with ANSYS.

Is ANSYS so much better to be worth the hassle? http://fsae.com/groupee_common/emoticons/icon_smile.gif

[fixitmattman]

I've never had any good luck importing any models from the usual CAD packages into Ansys. I don't use the program an extensive amount like I do the CAD packages so maybe I'm just doing it wrong. But even when I did get models to import my confidence in them wasn't there. Generally I just build my truss model from scratch in Ansys and work from there.

Cosmos is quite handy for general analysis and is not significantly less accurate, but as far as I'm aware Ansys is still for the most part the standard.

[DonMolina]

Originally posted by fixitmattman:

Cosmos is quite handy for general analysis and is not significantly less accurate, but as far as I'm aware Ansys is still for the most part the standard.

Well, ANSYS is undoubtedly one of the best solutions (if not THE best) for FEA.

But solving the frame is not something worth the trouble.

With Cosmos, you lose a totally insignificant amount of precision and you gain soooooo much in ease and speed and productivity that for me at least (and all of our team for that matter) there's not even a discussion on what package to use.

Being able to change your designs in a jiffy and have the results of a new study as fast, is what makes designs better imho. Trying to get the best of 2 designs never beats trying to take the best of 10 designs.

However, turns out that software is just like ladies (yes we engineers are THAT geeky unfortunately). Some of us like blondes, some of us go with the brunettes' option etc... http://fsae.com/groupee_common/emoticons/icon_biggrin.gif

[Wes Burk]

I agree with the COSMOSWorks beam-element study being ridiculously easy. It is my first year using the program and I can set up from scratch a study and solve it in a few minutes.

HOWEVER, last year we used ANSYS (i forget what beam element type) and the study matched our physical testing within a couple percent. Then when I studied the same frame model in COSMOSWorks it output consistnant torsional stiffness values 30-40% higher. We used a conversion factor to equate the ANSYS and COSMOS values because the ANSYS values matched our physical testing. Will be able to get to the bottom of it when we complete this years physical testing and do an ANSYS model of the new frame, but I was wondering if anyone knows how to manipulate the beam element tests in COSMOSWorks like how you can choose a different beam type in ANSYS.

[eklipse]

I still didn't seem to get an answer to my questions over the weekend.

Regardless, Ansys is a very powerful package and I have seen model iterations done in a matter of seconds with DesignExplorer - Design of Experiments. I would like to continue working with Ansys considering it is an industry standard and for its reliability.

Back to the purpose of the thread. Can anyone with experience in Workbench offer any useful advice on the questions that I have asked.

Somebody asked about an easy method for entering keypoints automatically in Ansys Workbench. Yes, you can make a table in excel and export it as a Comma Separated Values (CSV) file and import them. Take a look at this tutorial http://www.padtinc.com/epubs/f...1006/TheFocus_52.pdf (http://www.padtinc.com/epubs/focus/2006/0052_1006/TheFocus_52.pdf). If you look carefully you will find an FTP link to download the sample files.

Ansys workbench does analyze as solids however it automatically chooses your element types whereas you have to option to choose in Ansys Classic. If you click on FE Modeler you can view the element types if you look carefully. Typically, using Ansys classic, 2 point beam 188 elements will suffice. I would like to solve my analysis using lines and surfaces but I can't seem to change this option in Ansys Workbench, if anyone knows how to, it would be very helpful.

I still need to know how to constrain my beam lines to solid surfaces. I tried using a bonded connection however I can't seem to pick lines or keypoints, only surfaces. Can anyone help with this?

[RBbugBITme]

#1) It seems your nodes between beams are not attached even though they are at the same coordinate. There should be a merge function that will allow you to enter in a distance where all nodes within that distance will become one node and your beams will connect to each other.

Oh and any panels I wanted connected between tubes were modeled as shell elements. I would keep it simple and forget the solid model stuff you're doing in Ansys, at least during the initial testing to ball park your design.

[eklipse]

Ryan,

I found out that some of my lines needed to be split in my model because Ansys Workbench didn't recognize that there was a common keypoint at two intersecting lines. You can tell this is the case if a line leaves an intersection with the same color. This is one of the flaws of importing lines sketches from IGES files.

How do I convert my brackets to surfaces from solid bodies?

A friend of mine was able to use an MPC connection to connect a vertex/keypoint of a line to the surface of a solid body however I couldn't imitate the same action in Ansys Workbench 11. When I open his file, it's connected and it solves the solution before but it won't let me select vertices/keypoints when I try the same thing. Any ideas?

[RBbugBITme]

Ah yes, ran into that problem to. I actually stopped trying to import iges files after this and a few other problems and just wrote my own code which broke up all the element lists by tube size and all the Ansys nodes matched numerically and positionally to the nodes in the solid model which made it easy to switch back and forth.

With that said, I don't know how to handle your bracket issue and I also use ProE not Solidworks if that matters. I would assume your bracket has simple enough geometry it could be remodeled in Ansys and attached easily? Have you tried that?

[eklipse]

I have remodeled just a simple solid in Ansys Workbench just as a test and still cannot seem to make a Bonded Contact between a vertex (keypoint) and a surface body. Has anyone else had the same problem with Workbench before?

It could be an internal program error since as I mentioned before my friend was able to do it in his program, however, he is using Ansys Workbench 11.1, whereas I am using Ansys Workbench 11.0. As I said before, I got him to make the bonded contact between a vertex and a surface in his program and send it back to me. When I opened the file it showed a question mark next to the bonded contact feature and the Target Contact which says "Vertex" is highlighted yellow. Normally, it is only highlighted yellow when a selection hasn't been made and it will say "No Selection", however it shows an error with it selected as "Vertex". I can solve for the solution but cannot replicate the same bonded contact.

Has anyone else experienced this problem? Surely, I can't be the only one using Ansys Workbench for frame analysis experiencing this problem.

[Samo Simonian]

eklipse,

I'm not an expert but have had some fighting and loving with Ansys/workbench.

From what I know workbench will not want to make a contact between 1 vertex or edge and a surface. Apparentlty cannot model that. However the old ansys commands are still available, they're only called snippets now. Look for the icon of a text thingy with a red C trhough it (that is if you have the privilege of using that utility in workbench, if not contact ansys support or so). You can then insert traditional ansys code amidst your model tree in workbench. I imagine that in traditional you'd be able to just make a hard connection (MPC) betwee that 1 vertex and nodes on the respective surface? I havn't tried snippets yet, but the guy we got an ansys workbench course from said that it oughta work.

Additionally, Catia for instance has several options of saving a model to other formats. For instance STP IGES etc. and for STP you can again choose different types: line surface or volume. Maybe if you fiddle around with the type of file with which you save your chassis in CAD, Ansys might recognize surfaces and hence no contact problems.

No idea if this helps, good luck anyway.


Regards,

Samo

[Hotwheels]

Originally posted by eklipse:
I still didn't seem to get an answer to my questions over the weekend.

Regardless, Ansys is a very powerful package and I have seen model iterations done in a matter of seconds with DesignExplorer - Design of Experiments. I would like to continue working with Ansys considering it is an industry standard and for its reliability.

Back to the purpose of the thread. Can anyone with experience in Workbench offer any useful advice on the questions that I have asked.

Somebody asked about an easy method for entering keypoints automatically in Ansys Workbench. Yes, you can make a table in excel and export it as a Comma Separated Values (CSV) file and import them. Take a look at this tutorial http://www.padtinc.com/epubs/f...1006/TheFocus_52.pdf (http://www.padtinc.com/epubs/focus/2006/0052_1006/TheFocus_52.pdf). If you look carefully you will find an FTP link to download the sample files.

Ansys workbench does analyze as solids however it automatically chooses your element types whereas you have to option to choose in Ansys Classic. If you click on FE Modeler you can view the element types if you look carefully. Typically, using Ansys classic, 2 point beam 188 elements will suffice. I would like to solve my analysis using lines and surfaces but I can't seem to change this option in Ansys Workbench, if anyone knows how to, it would be very helpful.

I still need to know how to constrain my beam lines to solid surfaces. I tried using a bonded connection however I can't seem to pick lines or keypoints, only surfaces. Can anyone help with this?

Hi

I have used this method to import keypoints into the ANSYS Workbench Design Modeler. I'm having no problem generating my lines point to point and specifying the cross sections for the beam members as a whole.

What I don't know how to do is how to specify two different cross sections to two separate beam elements in the same space frame. I think i need to create more than one line body, but how do i do this?

Also how do I specify two different material properties for two different beam elements in the same space frame?

Also how did you specify the joints (vertices) to be rigid?

[Okan]

Here is your answer:

In "Design Modeller", you have to select (body) line bodies which you want to connect with each other, then right click and press "Form New Part". You can easily connect line bodies (even line bodies which have different cross sections) with doing this. But be sure that line bodies has to has at least one common point. In simulation, model will come with line bodies which are already connectted. You dont need to define any connection in simulation module.

[BeaverGuy]

Your first two problems really are the same.

As was mentioned Workbench does not allow contacts to be generated between vertices. As a result your model us undercontstrained and flying every where.

To create edge/face contacts you have to manually turn that on as an allowable option. The default is for only face/face contacts. This option will be in the details view of the connections item in the tree outline.

You can fix the additional uncontstrained areas two different ways.

The first is to import the model through design modeler and put all the bodies that are connected into a single body via form new part. Now select the bodies in the new part use the join tool in design modeler to designate joints between them. This causes bodies that are touching to share nodes so they don't need any connections. However, this will not work to connect shell or beam elements to solids because solid nodes only have 3 DOF while shell and beam elements have 6 DOF and if you try the solids will not show up in the simulation.

The second option is very similar to what you would do in the classic interface but can be time consuming. First you need to create a series of named selections. These are essentialy cm commands for the nodes of the body, face, edge, or vertex that you have selected. Now you need to add a command snippet in the boundary contidion portion of the simulation tree. The command snippet needs to start with:
/prep7

and end with:
allsel
/solu

in between will be series of cmsel commands and whatever constraint commpands, cp, cpintf, ceintf, rbe3, etc., That you want to use to tie the frame together. If you have a series of connections that are the same type you could sequentially number your named selections and then use a *do loop to go through them.

In all likelyhood you will have to use a combination of the two methods but if your model is setup with only shells or beams that touch then you can avoid using the command snippet. My recomendation if you do use either of these methods is to write an ansys input file and then read that into the classic interface to verify that your connections are correct and any joints generated in design modeler are maintained.

Some other information about elements
The default elements in workbench are
Shells: Shell181 a 4 noded shell, some properties can be defined with real constants but section commands allow more freedom
Solids: Solid186 20 noded 6 sided brick or Soild187 10 noded tetrahedron
Beams: beam188, 2 noded beam element can only be defined by section commands

However, you can force some solid elements to become different elements. If you have only 6 sided bricks and select the drop midsid nodes option you will get solid185 elements which are 8 node bricks instead of solid186 elements. Also, if you use a sweep method in the meshing and automatic thin model option some solid elements will mesh as solsh190 which are 8 node solid elements that more accurately model plate structures than standard solids do.

Also, if you know the itype number you can change between elements with the same number of nodes and nodal dof using a command snippet. The only real use I have seen for this within workbench is if you want to use real constants to define a beam section instead of section properties. I have changed beam188 elemements into beam4 elements by issuing a kt,X,4 command where X was the itype number.

[Gogo]

Hello,
I examine a manometric membrane by using the Static Structural Analysis of Ansys Workbench. The analysis is done via the Quadratic Tetrahedron element by default. The major point is whether this element could be replaced with Shell41 and how it could be done with Workbench. I have attached a picture of the membrane.
http://www.sunnoclub.org/webdisk/Analisis.jpg

[The_Man]

Your link to the picture is broken, or I can not see it for some reason.

You will probably have to give more details about constraints and loading before anyone can really help you.

Switching from Quadratic Tetrahedron to Shell will not be straight forward(just changing the element type will not do) because you will be moving from 3D to 2D. Shell41 is suitable for pressure modeling though you shouldn't have a problem.

[Gogo]

I'd like to do an analysis of the characteristics of pressure-deformation of the manometric membrane through Ansys Workbench. I use the elements Pressure and Fixed Support of the Static Analysis as shown in the attached pictures.
http://sunnoclub.org/webdisk/Analysis-2.jpg
http://sunnoclub.org/webdisk/Analysis-3.jpg
How can I change the FEA element from Solid to Shell? Is there any option in Workbench, and how can I set it to make Nonlinear Structural Analysis? I don't have much experience with Ansys?
Thank you in advance.