Dynamic behaviour of vehicle´s chassis through simplified static analysis?

  • 123 Views
  • Last Post 2 weeks ago
  • Topic Is Solved
timescavenger posted this 4 weeks ago

Hi there,

I want to simulate the dynamic behaviour of a vehicle´s chassis, formed by an assembly of bolted beams, during a "braking while turning" maneuver and wonder whether it could be acceptably simplified with either of these two approaches rather than going for a transient or explicit dynamics analysis:

1.1. Static structural analysis setting the corresponding braking and centrifugal accelerations, besides gravity, with 6 DoF constraint in 3 points just to avoid rigid-body motion and inertia relief "on" to balance the applied accelerations.

1.2. Initial Rigid-Dynamics analysis to obtain maximum reaction forces and moments to be exported as motion-loads to a second conventional Static structural analysis.

Another involved issues are:

2. whether to simplify the geometry with midsurfaces to mesh with shell-elements or go directly for solid-shell elements from the original 3D solid model.: pro&cons of each option?

3. how to apply the weight of the non-modelled geometry of the vehicle´s bodywork,seats, passengers,etc. Here I intend to use remote boundary conditions scoped to the fixation areas in the frame and attached to the corresponding mass points located in the different centers of gravity... sounds good?

4. How to model the bolted connections and beam contacts? Related to this, is the Inertial Relief approach compatible with eventual nonlinearities introduced by beam contacts and bolt pretensions?

What do you reckon? How would you go about it anyway?

Any suggestions/hints will be welcome! Thanks in advance.

Order By: Standard | Newest | Votes
peteroznewman posted this 4 weeks ago

Years ago, I did some auto-cross racing in a parking lot. I was impressed to see cars lift one wheel off the ground while braking and turning and learned to do that myself. Is this the kind of result you are looking for?

1.1 Yes, use 6 displacement constraints on 3 points to do Static Structural. If X is forward, Y is lateral and Z is vertical, the car is turning left, and the left rear wheel is going to lift off during braking and turning, then the right front wheel has XYZ set to zero, the left front wheel has XZ set to zero and the right rear wheel has Z set to 0.  Then you apply the acceleration that is the combined gravity, turning and braking acceleration (or put them in separately).  There is no need for inertia relief in this setup.  You would use inertia relief if you put tire forces at the three points instead of displacement constraints.  The reaction forces at the three points will be the tire forces and will balance the acceleration forces.

1.2 You could use Rigid Dynamics to find the acceleration due to turning since it varies from the left to the right side of the car due to the turning radius, but as a first pass, you could skip this analysis and just apply a constant sideways acceleration in the 1.1 model.

2. Simplify with midsurfaces. You get fewer nodes and can use quadratic elements. With solsh190, you have to set the element Z axis to be in the thickness direction on the solid body.

3. Say the car and driver total mass is 1000 kg with all the parts. There are a few large point masses, like an engine 300 kg, a driver 100 kg, a transmission 100 kg and the frame structure has a mass of 100 kg. There is a non-structural, non-point, missing mass of 400 kg. Edit the density of the material of the frame and make it 5 times larger. Now the frame will have a mass of 500 kg, which is distributed over all the frame, and the total car mass will be 1000 kg.

4. Use Fixed Joints to model the bolted connections. You can probe the Joint to see the total force transmitted through that joint. A few separate, detailed models would be built for the few bolted connections that have high forces to evaluate in detail, using solid elements, what is happening at that connection. Not sure what you mean by beam contacts. You don't need Inertia Relief if you have fully constrained 6 DOF.

timescavenger posted this 4 weeks ago

Thanks a lot for your hints Peter. I can imagine that racing was fun!

Some comments on them:

1.1. In all examples and tutorials I could find and read about Inertia relief option, they mention the program automatically calculates the body accelerations needed to balance the applied forces and these always appear as such in the setups (very much the same you mention with reactions in tires) so I was confused about how to use it (and whether to do it all) if the only known data to input are the braking and turning accelerations... so if I understood you correctly, you don´t need inertia relief if there are no applied forces as such (and fictitious forces coming from accelerations like gravity and centrifugal/braking ones don´t count as such). But if you use it, will the outcome be the same or different (wrong if so, I suppose)? Still, if you introduce the reactions forces in the tires, will the analysis be more realistic or complete? What would the difference be? Moreover, how do you know/obtain these reaction forces anyway?

1.2. Also, would you introduce the turning sideways acceleration separately as a rotational velocity (in this case I suppose using the expected/foreseeable minimum turning radius for the axis definition) or somehow else?

My case is really a with 3-wheeled vehicle or, to be precise, just the sidecar of a motorcycle. I reckon I can adapt your suggestions for the 3 points (wheels) constraints to my case replacing the two left wheels for the attachment to the motorcycle frame... but if you think this specific case poses any special consideration to be taken into account please let me know!

2. I started trying with solsh190 with the idea of avoiding the tedious tricky work of converting the solid bodies to surfaces because the CAD geometry is quite dirty and also because there are some "non-midsurfacesable" solids anyway, but now I am realizing the work has to be done equally to clean and prepare the solids for the mesher to accept them as sweepable... besides I forgot about the condition "Z-axis in the thickness direction of solid bodies" so it was not working! How/where do you establish this? ...

Anyway, I might follow your suggestion and change the approach to shell-elements.

3. Got it! Same as before...

4. I already had in mind to do some submodelling to find out detailed behaviour of the most stressed joints as you suggest. By “beam contacts” I meant that I intended to model the areas where beams touch each other with frictional contacts (i.e. Nonlinear) together with the bolts themselves simplified as beam connections with a pretension applied to each of them (which would also lead to nonlinear analysis, wouldn´t it?). I assume you suggest a more simplified approach which will keep things linear, do you? Is it not worth to attempt the more detailed (but also more complicated) modelling?

Again, your feedback is much appreciated.

peteroznewman posted this 4 weeks ago

1.1 Here is the Simutech tips on Inertia Relief.  "The sum of the reaction forces at the constraint points will be zero." You don't want that. You actually want the reaction forces at the constraint points to be the tire forces and they will sum to a non-zero value, like F = ma.  You have a total mass and a total acceleration, and the tires have to support that with a total force of F at the constraints.

I don't agree with the SimuTech tip that says to apply sufficient constraints to prevent rigid body motion. That is not necessary, Inertia Relief is specifically useful for unrestrained models. Consider a piston engine. I had a spreadsheet for the velocity and acceleration of the piston as a function of crank angle and rpm.  Consider the connecting rod, the top bearing has a known vertical velocity and acceleration, the bottom bearing has a known tangential velocity and radial acceleration. You can get static equilibrium using Inertia Relief and the solution will calculate the body force and the forces at those two ends to put the whole model into static equilibrium.

1.2 The lateral acceleration generated by turning is significant. You can calculate what that is from the forward velocity of the car and the turning radius. You can put that and the forward deceleration due to braking and gravity as three accelerations.

For three wheels, using the same frame of reference (X forward, Z vertical), the front wheel has XYZ zero, the rear wheel has YZ zero and the side car wheel has Z zero.

4. There might be 100 beam connections in the frame. If you solve the model and find three have much higher forces going through them than the next 97, you will save some time using fixed joints for the 100 connections in a first model, then in a second model, replace three joints with more detailed connections.

timescavenger posted this 4 weeks ago

Thanks Peter,

Precisely this article by Simutech is one of those I consulted and it somehow confused me with sentences like the one you mention and others like "If there is enough constraint to prevent vertical motion, but the vertical load does not exactly match the weight, there will be strong reaction forces where the vertical constraint is applied ... Inertia Relief gets the FEA model to exactly balance the force difference (applied force minus weight) in a static analysis with acceleration body forces over the whole structure, so that the reaction on the vertical constraint is zero". In this other article I also read "Using Inertial relief in conjunction with Fixtures is NOT recommended, since the forces from the inertial relief are applied alongside the stabilizing load that a fixture applies, and thus may drastically influence the resultsInstead, it is recommended to apply inertial relief when anticipated forces applied by Fixtures are small or zero, and when the model is balanced by External Loads (with few exceptions)"

But, if you don´t need and don´t use Inertia relief at all for situations like this (which, from what I understood, is one of the typical cases for using it: aircrafts in flight, vehicles on test track and the like), how is it then a static analysis equivalent/assimilable to a dynamic one? and why do you need to just prevent rigid body motion restraining only 6DoF in 3 points and not using regular constraints? What this case should be like then for the inertia relief option to be required/applicable? maybe defining velocities and accelerations like in your engine rod example?

Sorry to insist but, all in all, I find this inertia relief issue quite confusing...

About all the other issues, I am with you: I appreciate your advice and I´ll go that way!

peteroznewman posted this 4 weeks ago

The method I outlined above is simplified. It begins with known accelerations, the lateral and braking accelerations, perhaps measured in a real car while driving.  It supports the frame in an exact constraint pattern, which leaves the frame free to deform and twist, subject to a few assumptions.

One assumption is that all three wheels remain on the ground.  In the example of a car with four wheels, you would monitor the Z displacement of the unconstrained wheel. If it dips below the ground, then you would add a zero Z constraint, since the acceleration is not enough to lift the wheel off the ground.

Other assumptions require a bit more thought.

Two of the three wheels (bike wheels) are supporting all the lateral Y forces, because there is no Y constraint on the third wheel.  To get the third wheel to support some lateral forces, you could apply the lateral force directly to that tire, assuming you know what that force is.

One of the three wheels (front wheel) is supporting all the braking X force. This is not strictly true but it is a good approximation. Most of the braking force is on the front tire. Again, if you know the tire force in the braking direction on the rear wheel, you can add that X force to the model at the rear axle.  You don't add the lateral force to the rear wheel because there is a Y constraint that will solve for the lateral force.

If you wanted to model Tokyo Drift driving, where the two rear wheels are slipping sideways, you know the limiting lateral force from the COF of the tire to the road when they are sliding. Apply those lateral forces to the rear wheels and delete the Y constraint but keep the Z constraint. Delete the applied lateral acceleration. Now the model is under constrained, there is a lateral force on the rear wheels, but nothing for it to push against, there is no Static Equilibrium. Turn on Inertia Relief and now the solver will solve for the lateral acceleration required to balance the lateral force on the rear wheels that represent tires slipping sideways.

timescavenger posted this 4 weeks ago

Nice guidelines. As soon as I get the geometry ready to be used (still struggling with some tricky dirty features) I will try to implement them and will let you know what I get. Meanwhile, thanks again for the valuable hints

timescavenger posted this 4 weeks ago

 

Hi again,

About the way to configure how geometry parts contact each other and what I meant by “beam contacts”: I think my point can be seen and understood clearly looking at this article: in enhancement nr.3 you see 3 bonded contacts (one of them for the bracket to base contact and the other two for the bolt to base and bolt to bracket). Besides they join bracket and base with an extra “fake bolt” using the beam-connection new feature which then, they explain, can be assigned a pretension like for a regular bolt, which is the new feature indeed.

Now my doubt/question: should the bracket-base contact be a frictionless or frictional one, I would understand this setup because the forces would transmit through the bolts (real or “fake" ) and the joined parts (nonlinear) contact just works to avoid bodies interpenetration, sliding, etc.

But, if the bracket-base contact is defined as bonded (which, as far as I understood, is equivalent to glued/welded surfaces) what is the point with adding bolts (real or fake) in specific points of these areas which are already connected in all their common nodes? Wouldn´t they just be redundant/useless? (I reckon this would be equally true for your suggested alternative (fixed joints), wouldn´t it?)

In other words, if you want to model the real working of the system (i.e. force transmission in specific points through bolts) but don't want to enter into complications from nonlinear contacts, what do you do with the parts areas in contact? Can you just delete and get rid of these contacts and assume/despise that the parts might interpenetrate? Or am I missing something else here?

The same doubt arises to me with the similar explanations in this other article where at the end of the same case (2. beam bolts) they seemed to start tackling this very question but the phrase appears uncomplete!!: “The contact between the mating plates is...”

In my case some frame profile-beams are welded and others just touching each other and bolted: I thought to model the former case with shared topology and the later with contacts+"bolts" (e.g. beam-connections) and then the whole issue explained above arose. I have a lot of areas with this situation in my assembly and don't figure out how to best deal with it...

peteroznewman posted this 4 weeks ago

I am currently building a structural model of a large machine that consists of welded sheet metal subassemblies bolted together. The sheet metal has been idealized to midsurfaces. I am using Beam connections to represent the bolts. I am not using any contact at the bolted joint. I want a linear model that will be subjected to a transient acceleration load that represents an earthquake. I am using a mixture of bonded contact to represent welds where two faces are overlapping, and mesh connections where the edge of one sheet is perpendicular to another sheet and there are welds at the tee intersection. This model will produce plots of stress in the sheet metal, and axial and shear forces at each beam. There may be 100 beams in this model, but it will solve quickly because all connections are linear, so a MSUP Transient solution can be used (or even faster, a Response Spectrum analysis).

Review of the results of this model may lead to a detailed model of a few of the joints that carried very high loads. In the detailed model, the beam is replaced with a 3D model of the fastener that can include pretension and nonlinear contact of the mating parts. The nonlinear contact will mean a Full Transient solution, which will take much longer to compute, but the few joints that carry the highest load will be modeled with higher fidelity.

You can use a similar strategy for the bike frame with sidecar if you want a Transient solution, but you started this discussion asking about a Static Structural solution.

timescavenger posted this 4 weeks ago

Hi Peter, sorry if I confused you: I do prefer to keep the problem within static linear analysis (if reasonable and possible). I like the approach you exposed and it is pretty much what I had in mind but, for the reasons I posed, I was not sure whether to avoid any kind of contact and work just with shared-topology for welded parts (instead of bonded contacts) and just beam-connections (no contacts at all) for bolted plates/beams was a good/aceptable idea. I understood this will be similar to what you are doing for your transient case (simplifying welded-joints with shared-topology only instead of bonded-contacts + mesh connections) so I assume it will also work for my linear static one, won´t it?

peteroznewman posted this 4 weeks ago

If you leave your frame as solid bodies, then you can use shared topology. I choose to midsurface my sheetmetal parts. Now where two solid faces used to touch at a flange with a cap plate, there is a one wall thickness gap. That is why I use Bonded Contact at that flange.  I set the Bonded Contact to use Shell Thickness and set the Formulation to MPC so I can see the bonds after the solution.

For internal stiffening plates, which don't reach the outer wrapped box by half a wall thickness, I used Mesh Connections, which moves the nodes on the internal plates out to the box midsurface and shares a node, just like shared topology would. I can check the connection by the edge color code.

To clarify, here is a zoomed in corner of the solid geometry and the midsurface geometry.

     

timescavenger posted this 4 weeks ago

FolIowing your suggestion I finally went for a combined midsurfaces and solids approach (some connecting rods like the ones you see in attached pictures are not suited to midsurface like the frame plates and beams) so I also plan to define some shell-to-solid elements bonded contacts where they join (using shell-thickness and MPC Formulation as well). Looks good? Any comments? Not sure whether the surfaces orientation are OK and how to set/flip them...

 

peteroznewman posted this 4 weeks ago

That looks like a good approach. I also use a mixture of sheets and solids.  When you mesh it, and set Edge Color to Connection and if you see red edges (meaning free) where you wanted a connection, then you should use Mesh Connections and pick a master face and slave edge. The slave nodes move toward the master.

For the ball and socket at the end of the connecting rod, you can leave out the ball solid and create a Joint type Spherical and scope the reference to the inside face of the connecting rod hole, and the mobile face to the component (not shown) that the rod is connecting to.

timescavenger posted this 4 weeks ago

Thanks Peter. I keep moving forward and will let you know.

timescavenger posted this 3 weeks ago

By the way, the ball and socket at the ends of connecting rods are meant to serve during frame assembly to compensate misalignments and tolerances and they join frame parts through bolts and nuts (see image). Once all of them are fixed they "freeze" each other in their position so, in fact, they don´t work as moving ball-joints...then, could I just set a bonded contact between the ball and the socket inner surface? What would be the difference?

Besides, when reviewing how to model these bolted joints, which I intended to do with connecting-beams as well, I had the doubt about how to set them and whether it is the best way to model them at all: if you scope the beam´s reference and mobile ends to holes in the side plates (2nd & 3rd images) then the rod end (ball and socket) would be left unconstrained, wouldn´t it? The same situation appears when more than 2 plates are to be joined through the same hole with only one bolt&nut: how do you attach/fix the middle plate(s)? Put differently, what do you think it’s the best way to go about these cases?

timescavenger posted this 3 weeks ago

Hi Peter, did you see my last post? Was my doubt clearly explained? Thanks

peteroznewman posted this 3 weeks ago

Sorry, I missed the last post, thanks for the bump.

On the two plates that have holes for a nut and bolt that will constrain the end of a strut, pick the two circular edges and create a Remote Point and name it RP-end1.  The Remote Point will be created at the center point between the two circles, which is exactly where you want it. Do the same on the two plates on the other end of the strut and name that Remote Point RP-end2.

Since the only real function of the strut is to set a fixed (but adjustable) distance between these two point, I would add a Spring, which can be found under the Connections folder.  You can choose the two Remote Points for the Reference and Mobile ends of the Spring.  The spring rate would be AE/L, where A is the cross-sectional area of the strut, E is Young's Modulus, and L is the length of the strut.  Suppress the Strut parts in the model, you don't need them. Because it is a spring, each end acts like a Spherical Joint.

If you want to allocate the mass of that strut, you can add a point mass to each Remote Point that is half the mass of the strut.

When I have three plates that are bolted together by a bolt and nut through three holes, I would add a Beam connection, where I choose one circle for the Reference end of the beam and two circles for the Mobile end of the beam (assuming you have used midsurface on the plates).

timescavenger posted this 3 weeks ago

1. I see your point for the strut I represented although its cross-section is not constant since it is hollow in the centre but solid at its ends due to the threaded ball&socket ends (which I intended to model with a bonded contact between the strut-shell elements and the ball&socket solid elements). Besides, there are another 2 connections which are not straight struts but "Y-tube connections" with one end threaded to a ball&socket and the other two welded to the plate (image1)... so I guess the "spring solution" would not serve in this case, or is there still a way to somehow simplify it?

2. Applying your suggestion to join several plates with the same bolt&nut in one of my connections leads to this setup (image2) where the beam is represented ending between two plates at one end and between three plates at the other. Is this what you meant? Would that setup be ok?

peteroznewman posted this 3 weeks ago

1. The simple model of the Y-tube support for the threaded eye-bolt, create the Remote Point for one end of the strut at the hole in the eye, and scope that to the circular end of the tube midsurface. Then suppress the eye-bolt. 

I understand the strut is not a simple rod, but you just need a rough estimate for its axial stiffness. If you want a close estimate, you could mesh just the strut with solid elements, use bonded contact at the threads, fix one end and pull on the other end with a force: F, measure the displacement of the end: x, and compute the spring stiffness from k = F/x and not have to use solid elements in the model to represent the strut.

2. You have a correct beam. There is a hidden spider of connection elements from the beam end to the three circles at one end and the two circles to the other end of the beam.

timescavenger posted this 3 weeks ago

Probably just a stupid question but, since the ball&socket joints get "blocked" with the bolts&nuts, how can you be sure the struts work only axially and don´t support any bending/torsional load? I´ve been trying to figure this out and do not see it clear... Sorry if this is a bit missing the point.

peteroznewman posted this 3 weeks ago

After a simulation, you have solved for the deformation of the frame, using a stiff spring for the strut. Export the deformed shape of the frame as an STL and import that into the CAD system. Take a copy of the 3D strut with the nuts and bolts and align that with the two points in the frame and check for interference. 

timescavenger posted this 3 weeks ago

Thanks Peter. I will do it (when I can get back to it: now I must leave it for another more urgent matter) and I will let you know.

timescavenger posted this 2 weeks ago

Hi Peter, I could finally get back to my case. I followed all the hints we discussed so far and I think I already have it set up but when I try to mesh the assembly I get these error messages and don´t know why. I am stuck here. What are they and how can you fix them?

timescavenger posted this 2 weeks ago

Hi again Peter,

Somehow I finally managed to mesh the assembly: I am not sure I did it right or whether this was the thing to do and why it worked but using a Virtual-Topology object in the offending geometry highlighted from the previous error messages, I could obtained a pretty good mesh (at least that's what I think from the quality metrics):

Still, I am stuck: now the solver says there are hundreds of errors! but it doesn´t not specify which are they or where they are:

What could I do? Help!... and thanks again

peteroznewman posted this 2 weeks ago

These warnings are because you have quadratic shell elements that are being wrapped around a tube and there is apparently a limit to the radius of curvature to thickness ratio.

There are two ways around this. 1) Use smaller quadratic elements, which will reduce the extent of the wrap.  2) Change the Mesh to use Linear elements. These don't wrap, they have straight sides.  You might have to apply 1) and 2) to eliminate the element shape warnings because a quad element, if it is at a 45 degree angle to the tube will be twisted or warped, and there is a limit to warping, but the mesher will try to avoid that. To eliminate that problem, you can apply method 3) Use a mesh control to force triangles instead of quad elements. Linear triangles are flat, so they can't warp.

timescavenger posted this 2 weeks ago

I just let the program to control midside nodes instead of forcing to keep them as before and decreased the elements size and the warnings disappeared but now other errors show up although I restrained the 6 dof in the 3 points (wheels axis) as you proposed...:

Is there a way I could send you the solve.out and/or file0.err files? (the platform does not allow me to attach them: it tells me "file extension not allowed") because I see other weird warnings which make me doubt about the whole thing and would appreciate it if you could tell me whether you see something odd or wrong.

 

peteroznewman posted this 2 weeks ago

You can always attach .zip files, so put anything you want in that.  But I don't want the files you mention, I want to see the entire project.

You can always attach .wbpz files. This is one file that contains your entire project. Here are more details. Note the file size limit for any attachment is 120 MB. If the archive is larger than that, you can clear generated data on the mesh and save that. It will be smaller.

timescavenger posted this 2 weeks ago

 Fair enough! There you are (I translated some names to english for an easier understanding...). Please let me know how do you see it. Thanks

Attached Files

peteroznewman posted this 2 weeks ago

Got it, I will look at the model later today.

timescavenger posted this 2 weeks ago

Great. Thank you 

peteroznewman posted this 2 weeks ago

 1) Under Mesh, change Capture Curvature from Yes to No, that will make a smaller model, 120k elements instead of 437k elements.

2) Run a Modal analysis first to check that all the parts are connected.

The result shows that there is at least one piece and maybe 3 pieces of the tubos that is not connected to the rest of the tubos.

You have to repair that before the Static Structural will work. I think it is these three holes that somehow have a mesh across the hole. This seems like a software defect to me. Try using SpaceClaim to cut that section of pipe out of the frame and use mesh connections to stitch it back in as a workaround to this software defect.

Show More Posts
Close