Chassis Analysis with Hyperworks

[B. Gavin Potts]

Hello,

First post on the forum here. I have used Solidworks beam analysis to run torsion simulations for my Universities FSAE team for 2 years now. We have had good success matching simulation results with testing in terms of frame torsion. The problem is we use bonded composite shear panels which needs some more sophisticated FEA. Anyways, we have followed the tutorial put out by Altair on FSAE Tube Frame analysis which we have gotten our frame to run the analysis. The problem is there are a few nodes were the elements are not transmitting load which causes some very large displacement. We are using the 1D beam analysis and if you go to Tools/Check Elems/free 1-d's, it shows a few meshed elements that are "free". We have done a bunch of work trying to redraw the line using Hyperworks tools to ensure the node is proper. Then we looked at combining/cleaning up the mesh which did nothing in the end.

Next, the tutorial setups up the frame with uniform cross section on all tubes. To apply the correct tube sizes, we made different meshes from the imported geometry for each individual tube size(mesh1=1.00x0.095,mesh2=1.00x0.065,etc). We then created seperate properties that applied each hyperbeam tube section to the proper mesh. This all worked great but in the end caused even more of these "free 1-d's".

Does anyone have any suggestions or has used Hyperworks more extensively? We have tried to go through Hyperworks in which they blew us off and no one at our University seems to use the software.

Thanks for any help,
Gavin

[billywight]

Are you getting free 1D's because you have two or more nodes that should be connected (i.e. one right on top of another), or is it for some other reason? If the former, you need to equivalence the nodes. Tools - Edges - Change the selector to elements - select all (or whatever needs to be equivalenced) - enter a tolerance (perhaps 1mm or so depending on your element size) - click on preview equivalence. Brown dots represent multiple nodes within the tolerance sphere. If it looks correct, click equivalence and they will become the same node rather than multiple nodes in the same spot.

[Moop]

It sounds like you have unconnected, coincident nodes, and as Billy said, the edges panel will let you fix it.

There's an option to allow you to select nodes that are on top of each other, so you can see for sure that this is the problem. Hit O to open up the options panel, click on the graphics tab and select "coincident picking". Now, if you say hit F4 to grab the measure tool, when you go to pick a node, if there are multiple nodes on top of each other, you'll see a little circle pop up and it'll have numbers indicating the numbers of all the nodes that are there.

Sometimes, say when you're using connector elements, you need to have multiple nodes on top of each other, so you need to turn on coincident picking if you want any hope in hell of getting the elements all connected up properly.

[B. Gavin Potts]

Billywight,

I used your solution for the equivalence but what is that really doing? So there are two double nodes and this tool is just combining them? The terminology of "equivalence" does not tell you much. Last question, as I increase the tolerance to say 100, many more nodes on the frame show up as double nodes. Is this something I should use the equivalent tool on or just nodes that fail in my simulation?

Moop,

I did not get your method to work. I opened up the options menu after changing the graphics setting and when I click on the failed nodes, they just show up as green and blue. Any suggestions?

Another question for everyone that we have been debating is how the mock suspension is restrained/interacts with the frame. We created a new component for the suspension, made an rbe2 element representing the lower suspension along with a seperate rbe2 element representing the upper suspension and the upright. My question is how these nodes react to forces. When I apply an upward force for torsion, the suspension being a four bar linkage in the model should move up with no shock or pullrod modeled. Instead, the rigid bodies do not move which I am wondering how this interacts with the frame. What I am afraid of is if the rigid bodies are artificially constraining the front suspension notes or giving them extra support that will resist deformation under torsion. Sorry if I am not clear!

Thanks again,
Gavin

[Moop]

Gavin,

What the equivalence feature in the edges panel is doing is looking for nodes that are close to each other within the distance tolerance you specify and if there are any, it merges or "equivalences" the nodes.

When you increase the tolerance up to 100 mm, for each node, it's looking to find any other nodes that are within 100 mm. If you have any tubes less than 100 mm long, then hitting equivalence will merge those nodes and destroy your tubes.

If you're seeing them as green and blue, then you didn't turn on coincident picking. That or there are no coincident nodes at that point. For some silly reason, every time you close HyperMesh on our computers you have to reset the coincident picking option.

Anyways, to demonstrate, I opened up HyperMesh and made two nodes at (0,0,0). After turning on coincident picking and trying to select the node(it doesn't have to be the measure tool, any panel that's asking you to select a node will do. F4 is just really easy to hit with my pointer finger!), you'll see this:
http://s14.postimage.org/w10u8y6wd/coincidentnodes.png

You can now click on either node 1 or 2 to select it. You'll need to be able to keep this straight to use connector elements. Thankfully, if you have any elements connected to these nodes, when you mouse over the node, HyperMesh will highlight those elements white.

The way you have it defined right now, your suspension arms are basically rigid beams welded your chassis. To allow your suspension arms to move, what you will need to do is either release the rotational DoF at the nodes where your suspension arms connect or use balljoint connector elements between your arms and frame and arms and upright. It's probably a better idea to use connector elements, as what you've done is more easily visible to the next person that opens up the model and it's easier to find the options in HyperMesh to setup connectors than release DoF of beam elements

As you said RBE2, I'm assuming you're solving with NASTRAN? I'm not familiar with the connnector elements in NASTRAN(ABAQUS is what I know), but you should be able to look in the documentation to find which connector element you want. You want the one that restrains all translational DoF between the two nodes but releases the rotational ones. It's called a JOIN connector in ABAQUS.

For some silly reason, Altair decided to hide connector elements under the rods panel, and the default element that the rods panel creates is a truss element(at least in ABAQUS). You'll have to go to the elem types panel, click on rod, change it to whatever the connector element name is in NASTRAN(it's CONN3D2 in ABAQUS), and then you can go back to the rods panel to create your connector elements. You'll then have to create a property for your connector elements. I don't know how properties are defined in NASTRAN, so you'll have to figure out from the NASTRAN and HyperWorks documentation how to get that setup.

Hope this helps

[B. Gavin Potts]

Moop,

After going back and playing with that function, it works great now.

The first time I setup this model, I created one mesh of all the tubes and then selected each element by hand(took ages) and assigned it to a separate property for each tube size. What I tried to do was create a mesh of each tube size because you can just select the geometry lines and then create an individual property for each of those meshes. For some reason, I get an error when running this model that says something about this is continuation line 1 of PBEAML, 1 bulk data. It seems like it has an issue with my beam section that I created because bellow that it says + 10.0287 0.0 which is the inner radius of the first beam section I created. The other thing I am thinking is there something you have to do between different meshes like a connection because previously I had one single mesh with different properties and now I have 5 mesh components and 5 properties. Any thoughts?

Thanks again,
Gavin

[Moop]

Gavin,

From a model clarity standpoint, you definitely should not have all the elements in one component. The way we have it setup is we have a component for each tube cross section, make sure the proper tubes are in the proper components and we then assign the element property for each tube cross section to the entire component. I'm not sure what you mean by assigning properties to the geometry lines? Have you assigned the properties you created to the components you created?

Depending on what version/update of HyperMesh you're using, you can right click on the component in the model browser and click on Assign. If the option isn't there, you can click on the Components button on the Collectors toolbar, hit the assign radio button and use that to assign properties directly to the component. You can assign properties to elements directly but it's a lot more difficult to track what is doing what.

I'm not sure if it's possible to accidentally assign multiple properties to the same element. This could be the problem you're seeing, although I would think the error message would indicate that pretty clearly if this was the case.

As I said, I don't know NASTRAN very well so I can't be super helpful with sorting out errors in the deck. I'd check and make sure that all your components have a property assigned to them, and check with the NASTRAN documentation to make sure you're inputting your cross section information properly. The NASTRAN documentation should have some examples that you can read through that will show you sample deck output for example problems. This will let you see how your beam sections should be defined in the deck and how it says in the deck which properties are assigned with which elements. This way, you can read through your own deck and see where the trouble is. And if you have any square cross sections, you should be able to find out how to tell it the cross section orientation. Any square tubes you have will probably be oriented so that the flat sides are verticalish, so you should only need one property to define these beam sections.

Once you learn how to read the deck, it's usually easier to find where the problem in your model is by reading through the deck than looking through your model(unless it's some sort of element quality/geometry issue which you obviously can't see in text, haha). You'll want to get something better than notepad though. I'm not sure how it's setup in NASTRAN decks, but for ABAQUS, all of the keywords are preceded by a *. I use Notepad++ for this because it's free, and what I do is ctrl-F to find all of the *'s in the deck, and it brings back a list of all the lines where there's a * and lets you click on the list to jump to all the keywords. This way you can quickly read through your deck, since the only parts of it you actually need to read are the 50 or so lines with or right after keywords.

You won't have to make any connections or anything between elements in different components. As long as the elements have the same nodes, they'll be connected. This will be more apparent if you take a look at the deck HyperMesh spits out. You'll see it just lists a bunch of nodes(or grids as they call them in NASTRAN I think?), and then when it defines your elements, it'll reference those node numbers. Basically, all the components are there for is so that HyperMesh can use them to group elements together and easily create sets of elements that it can then use to tell the solver that all of the elements in this set have this property.

Actually, you might be SoL on the easy searching through the deck. I just looked through an OptiStruct deck, which as far as I know is almost identical to NASTRAN, and it doesn't seem to be easily delimited like it is in ABAQUS. It also seems that instead of named element sets(HyperMesh makes take on the names of your components for easy deck reading), it uses numbers to indicate element sets for each element and then in the property line, it gives the element set number that the property should be assigned to. Although you might be able to make use of the comments that HyperMesh puts in with $'s

If you don't find any problems with how your properties are defined ans assigned, it may be easier if there's somebody at your school who has experience with NASTRAN. They should be able to read your deck and tell you what's wrong pretty easily.

[B. Gavin Potts]

Moop,

I appreciate these responses, they are extremely helpful. I am working on the NASTRAN/Abaqus deck that you mentioned. I have never read into those files before but I just exported both the Nastran and Abaqus decks to compare them(just using notepad for now). They generally show the same in info from what I can see, just a little different format. This is the section under Property Definition for Surface and Volume Elements for the model that is not working.

$$ PBEAML Data
$
$HMNAME PROP 1"1.00x0.095" 3
$HWCOLOR PROP 1 49
$HMBEAMSEC PBEAMLASSOC 1 1
PBEAML 1 1 TUBE +
+ 10.287 0.0

On the other side, this is the same bit from the model that has all 1D mesh as a single component and assigned to different properties for tube size.

$
$HMNAME PROP 5"1 X .095" 3
$HWCOLOR PROP 5 1
$HMBEAMSEC PBEAMLASSOC 5 5
PBEAML 5 1 TUBE +
+ 25.4 10.287 0.0

It seems like it is not including the 25.4 mm diameter column into my latest model. I checked in the hyperbeam input and it is correct there. I then went into the Property card image and it shows up properly with DIM1A and DIM2A and NSM 0.0 but for some reason this information is not being exported to the deck. I feel like the model is setup correctly but the PBEAML dimensions are not transferring over. In the last hour, I started the model from scratch with the same result. Any thoughts?

Thanks again,
Gavin

[B. Gavin Potts]

Corretion! After clicking around enough times I guess it just falls into place sometimes. I think what happened was I created folders and beam sections in hyperbeam. I noticed that some of the inner and out diameters were coming through on the nastran deck but some were not. After some messing around, it turns out if you go to the card edit, click beamsec and then manually select the beam section. It is odd because before going through this process, the card image states that it is a TUBE with the correct dimensions so I just assumed the beam section was assigned to this property. Very odd.

Anyways, I appreciate the help and I hate to say it but I will likely be posting some more questions over the next few weeks. The end goal is to design a composite monocoque frame for next year’s car. I have been doing an independ study with another team member were we have learned a ton about laminate plate theory, layed up prepreg panels and are in the process of testing them at a local sponsor. We want to correlate that test data with the laminated plate theory and also Hyperworks composite FEA as a starting point to doing torsion testing on a monocoque frame. We want the design process to be theory based instead of just over building a composite frame and figuring out later where we can cut the fat. Going backwards, we do currently run bonded composite shear panels in our chassis but I have never modeled the panels and tried to actually design them in versus just adding them in later for stiffness.
I have setup a few models with the composites tools which are pretty slick. I would say the next part for me is to input the push rod/shock/bellcrank assembly and investigate the degrees of freedom to allow at each corner to more realistically simulate our real life torsion rig. Then, the question is how to mimic a glue joint from the composite panel to the steel frame. I have read a bit about connections which seem promising. Anyways, thanks again.

Gavin

[B. Gavin Potts]

Hello all again,

I was wondering if anyone had any theory on how to structure a suspension in Hyperworks? Basically, I have a rear subframe in which I am applying engine and differential forces and would also like to add the effects of the suspension pickups and also the bellcrank/shock nodes. I have been playing around with using RBE2 elements with not much luck. I have gotten the RBE2 elements to work in my torsion model but I feel like they could be restraining the subframe in ways I might not want.(Still needs more testing and thought) I have gotten a smaller scale lower a arm with vertical spring to show that CROD's can be connected to a CBEAML element and still rotate as if it was a ball joint.

At the end of it, I guess I am trying to use a node as a ball joint so the node will mode with where ever the frame deforms to but also holds the suspension member to that node. This is especially a problem when trying to get the bell crank to rotate. Is it as simple as just using rods and beams and tweaking the DOF or does it really require a multi body model? Once again, I appreciate all the input!

Thanks,
Gavin

[billywight]

Yes, I have done it before. You can create a linkage mechanism with a combination of rods, beams, and RBE2's. For the beams, you will likely need to create some coordinate systems to assign to the elements so the correct end releases are applied. Use a spring element or similar for the shock to check that the motion is working as planned before continuing the analysis (and of course replace the spring with a rigid for the actual analysis).

[Moop]

As I said before, you can accomplish this by releasing the correct DoF at the nodes of the beam elements representing your suspension components, or by using connector elements. I prefer connector elements, because I find them easier to set up/debug and because when the next person has to open your model, it's much clearer that there are some DoF released when they see CONN3D2(or whatever the connector element name is in NASTRAN) next to all of the suspension joints, as opposed to having to dig to find exactly which DoF are released for each single beam element.

At least, NASTRAN should have connector elements? Maybe it doesn't, I've never used it. Again, the documentation will tell you this and how to use them

[Drew Price]

Attention new members: ^^^ THIS is how to start a new thread. This is both helpful and insightful, and some very smart people are lending their expertise to assist someone who has gone through their due diligence trying to sort out their issue on their own.

It's refreshing to read a thread here and learn something I didn't know about.

[B. Gavin Potts]

Billywight,

I setup a simple model with just the lower a arm with a pushrod going into a constrained spring. I had a frame using CBEAMS that was constrained at the middle of the car roughly, then at the suspension nodes I ran CROD's out the pushrod point. After some messing around, I did get the spring to compress. One thing that is odd is that the spring can only deflect in 1 direction. This works fine if your shocks run a long an axis but in most cases this wont work. Can you fix this by assigning the vector orientation in the spring menu? I tried to assign a vector between the two nodes of the shock but the result did not change. Ultimately, something is keeping the shock from rotation but at no point did I assign DOF for the shock or the CROD. A way I checked this was to orient the force going downwards in which you would assume the pullrod would stay in line with the shock as it goes through the motion. In my case, the spring does not rotate so the pull rod and shock are no longer in line by the bottom of the travel.

Added note, I just tried to create a system that is from the shock constraint point that will in theory keep the y axis inline with the pullrod. My hope was to assign this new system to the spring and allow DOF 2 to allow it to deflect along that new system axis. It seems there is only a selector for vectors in the spring menu so this is another dead end..

Moop,

I currently have the rear subframe setup with CBEAML elements and constrained on the opposite side of the car in all 6 DOF. I then created an upper and lower a arm section from CRODS in which I made out of steel, tweeking the modulus up to make it ~infinitely stiff. I then connected the top and bottom a arm ball joints or what would represent the upright with an RBE2 element with all DOF restrained. If I run my pushrod straight to my shock, the shock does deform and the suspension moves. The problem I am having is with the bellcrank. I tried a series of RBE2 elements with CBEAMS and CRODs, just many different configurations and still have not gotten the shock to compress/elongate. Any suggestions? For some reason, the DOF when things are moving and rotating just is not settling with me.

Also, I did a few tutorials and watched some webinars on connectors. When would this be applicable for the suspension nodes? For example, if I have a CROD(a arm) going to the CBEAML(frame), this will behave like a rod end because the CROD is only delivering the axial force from the a arm. A situation where I could maybe see using the connectors is if you wanted to model the complete suspension using CBEAML's, but the problem being if you have a CBEAM to a CBEAM, this will freeze the joint and allow no motion. Again, I have not had muck luck with the pina/pinb in the bar sections but I am thinking you could achieve the motion using this method. In your previous comment, I think this is what you were referring to avoiding because it makes it difficult to go back and see what DOF you have selected. Is there a way to show on screen for each element its DOF? Back to the connector part, how would this apply to an a arm. Sorry if the comments are a bit redundant, I think once I get the DOF sorted out, this will all be much more clear.

Thanks,
Gavin

[B. Gavin Potts]

Drew Price,

Thanks the comment. I have gone through the forums trying to pick up chassis information for around 2 years now. As I mentioned earlier, my group member and myself chose to use HyperWorks for our composite project because many sources told us that the visualization tools are top notch for composites. Again, I have not used Ansys or Abaqus extensively so maybe others could give more insight on that. But the negative of using Hyperworks is the lack of help we have found around campus, intern jobs, etc. For some reason, we have only spoken to one person in Minnesota that has come across it! Anyways, we have worked with the software over the summer to get basic laminates tested but just in the last few weeks have been trying to model the frame. We really got nailed at Michigan last year for not having much justification on frame design besides torsion testing. That will not be a problem again this year!

Gavin

[B. Gavin Potts]

Hey,

I was wondering if anyone had read my previous comment about bellcrank and connector problem I have been having in HyperWorks. I have been spending way too much time in the last 3 days trying to figure it out with no luck. Once again, any help is appreciated!

On another note, I have been trying to model our composite shear panels as a 2D mesh in the frame model. Any suggestions on how to simulate the glue joint? I was thinking about offsetting the 2D mesh the radius of the tube, as how we would do it in the real frame and then use a connector around the perimeter from the 1D frame mesh to the 2D panel mesh. I still need to get this to work on a small scale before I apply it to a frame but any ideas or tips would be helpful.

Thanks again,
Gavin

[billywight]

Hi Gavin,

Shoot me an email and I'll reply with a .hm file so you can check out how I did the rocker.

billy(at)luxonengineering(dot)com