Issues with Static Structural Simulation of a Multi-Leaf Spring

  • 208 Views
  • Last Post 01 March 2020
  • Topic Is Solved
Samyak97 posted this 12 February 2020

I am trying to do structural simulation of a multi-leaf spring spring. I used remote displacement with one eye end(fixed end) of the master leaf to have rotation only about X and the other eye end of the master leaf(shackle end) to have rotation about X and translation about Z. I also applied load at the face of the smallest graduated leaf of the leaf spring. ANSYS shows a warning:

Not enough constraints appear to be applied to prevent rigid body motion.  This may lead to solution warnings or errors.  Check results carefully."

ANSYS calculates the values like total deformation (when all the contacts are bonded) but those it values are very unrealistic and incorrect. If i change the contact type to any other type other than bonded it shows solver pivot error. How do I solve this ? Please help

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 12 February 2020

I see in the image that there is a bolt though the springs. I expect there is one on each side of the center of the leafs and that the spring assembly is symmetric. You can leave the bolt in the model, and actually compress the springs at the bolt using a bolt pretension load as a first step in a two-step analysis, but for your first model, suppress the bolt solids and leave that detail out of the model. You can put it back in later if you want.

I recommend you go back to CAD and create two planes, one through the center of the length of the spring, and one through the center of the depth of the spring. If the geometry is in DesignModeler, you can insert a Symmetry object into the model and it will slice the solid bodies in those planes and just bring over a 1/4 model complete with a Symmetry object into Mechanical.

If you are in a different CAD system, make the cuts and just bring over 1/4 of each body.  Now on every cut face that has a Z-axis normal, create a displacement constraint of Z = 0 and on every cut face that has a Y-axis normal, create a displacement constraint of X = 0.  Those are your Symmetry boundary conditions for solid elements. This means the bodies can only travel in the Y direction, making the job of the solver much easier.

You had a good arrangement for the ends of the spring, but in the 1/4 symmetry model, the center plane doesn't move along X, so the end of the spring needs that freedom. That means the one remote displacement is like you had on one end, all fixed at 0 by Free in Z displacement.

In meshing, make sure you have at least two elements through the thickness of each leaf.

Choose the cut face of the smallest leaf to apply the load to. I recommend you choose a remote displacement, and you only need to specify a Y displacement.  Insert a Force Reaction Probe into the Solution branch and select that remote displacement to see the force vs. deflection curve. Displacement inputs make the job of solving easier than Force inputs.  Because you have only 1/4 of the material, it will only be generating 1/4 of the force at each increment of displacement, so multiply the Force Reaction by 4 to get the force that the full model would have delivered.

You need each spring leaf to have frictional contact working at the beginning of the solution. To do that, insert a Contact Tool under the Connections folder and Evaluate Initial Contact Status.  Look at the table it produces. Each contact must show as Closed. If any show as Near Open, then the solver will fail with a pivot error.  To fix that, edit the offending Contact and in the Details window, near the bottom is Geometry Modification where it says Offset, change that to Adjust to Touch. Now the contact is closed.

Finally, help the solver to find equilibrium. Under Analysis Settings, set Auto Time Stepping to On, set the Initial substeps to 100 (you can use a smaller number next time if it easily solves), and the Maximum substeps to 200. The minimum substeps can be 1 unless it has difficulty after the beginning. Most importantly, set the Large Deflection to On.

While the solver is working, look at the Newton-Raphson Force Residual plot under the Solution Information folder.

  • Liked by
  • Samyak97
Samyak97 posted this 12 February 2020

 

Sir, the leaf spring will only be symmetrical about the plane passing through the center of the spring (left side symmetrical to right side). The model of the leaf spring is based on the rear leaf spring of Tata Ace minitruck and the bolt-nut are a little offset from the center of the spring. What should be the preload value for bolt pretension? And also how much should we put as the value of coefficient of friction if we have frictional contact between the leaves.

Any help is appreciated...Thank you for your time.

Samyak97 posted this 12 February 2020

Sir, from the photo i have given before, the contact table shows some penetration. Sholudnt the penetration be zero, as the leaves should slide with respect to each other?

peteroznewman posted this 12 February 2020

I only see two Frictional contacts, but it looks like there are four layers to the assembly, so there should be three Frictional contacts. Use a value of 0.2 for the coefficient of friction. You can run the model two more times and see the effect of setting the friction to 0 and to 0.4 to learn the sensitivity of the force to the coefficient of friction.

What is the size of the bolt going through the leafs?  Use Bonded Contact of the bolt head to one face, bonded contact of the nut flat to the opposite face.  You must go into CAD and split the cylindrical face of the bolt shaft at the plane of the nut. Then you use bonded contact of the shaft face to the nut face.  The other part of the shaft cylindrical face gets the Bolt Pretension load.  Try 10,000 N as a start value.  This has to be applied in step 1, then the bolt pretension is set to Lock in step 2.  Step 2 is when the force or displacement is applied to the center of the assembly.

Samyak97 posted this 12 February 2020

Ok Sir, I added the third frictional conatct. What about the penetration?How to resolve that?

 The material used for the leaf spring is :

SAE 6150/ AISI 6150/ BS. EN47/ JIS SUP10M/ JIS SUP9/ DIN 1.8159/ 50CrV4

According to me, the load to be applied to the smallest leaf(as calculated) should be 5454 N

peteroznewman posted this 12 February 2020

When the solver starts, it will resolve the penetration as part of the solution process.

Samyak97 posted this 12 February 2020

i am facing these errors.

peteroznewman posted this 12 February 2020

Please create a workbench project archive .wbpz file and attach it to your post above.

There are many posts for Unable to Converge.  You can read a few while you are waiting for me to look at this model.

Samyak97 posted this 12 February 2020

Sir, I have posted the workbench project archive before your comment:

"When the solver starts, it will resolve the penetration as part of the solution process."

peteroznewman posted this 13 February 2020

If you delete the edge blends on the solid bodies before you bring them into Mechanical, you will get a more efficient mesh filling these leaf springs.

Without touching the geometry, just by setting the Mesh Defeaturing size appropriately, I can eliminate the blended edge.

The bolt does not stand up straight like this, it should be aligned with the surfaces it is clamping.

I recommend you delete the bolt and nut and the four holes in the leafs, delete the edge blends, and make the 1/4 symmetry model produce some useful results.

Then you can go back and make a more sophisticated model.

 

  • Liked by
  • Samyak97
Samyak97 posted this 15 February 2020

Sir, how is 1/4 th model possible here?

 I am getting this error.

also the errors which are consistent:

"Not enough constraints appear to be applied to prevent rigid body motion.  This may lead to solution warnings or errors.  Check results carefully."

"The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose."

 Even after setting geometric modification as Adjust to touch the solver pivot error is coming.

 

 

Attached Files

peteroznewman posted this 15 February 2020

Full model and Quarter Model.

Samyak97 posted this 15 February 2020

The remote displacement is not of the same kind on both the eyes as one eye is fixed and the other eye hinges about a shackle. Then how will the quarter model account for that?

 And also, i am not able to resolve errors, especially solver pivot error even after changing the geometric modification to "Adjust to touch" in the details window. Please help

peteroznewman posted this 15 February 2020

The XY symmetry BC prevents those faces from leaving the XY plane. That BC has "replaced" the fixed end of the spring that was cut off.  The remaining eye end should have a remote displacement with all DOF set to 0 except for the Z displacement and Rotation X, which should be left Free. That simulates the hinging about the shackle.

You can also use the face on the XY plane of the lowest leaf to apply the force at the center of the spring. This more accurately represents how the shaft is connected to the spring than applying it to the entire bottom face of the lowest link.

  • Liked by
  • Samyak97
peteroznewman posted this 15 February 2020

Make sure to put two elements through the thickness of each leaf.

  • Liked by
  • Samyak97
Samyak97 posted this 17 February 2020

Please have a look at the file please. I have corrected the hole alignment to the centre of the leaf spring and also used bolt pretension of 2000 N. I am no longer getting solver pivot error.

But i am getting some other errors:

Please have a look carefully. I have attached that file. Thank you for your time. 

I have also done the simulation with quarter model. I am attaching that also below. I am not getting any errors in the quarter model but the values of deformation do not seem to be reasonable at all. Please check.

Attached Files

peteroznewman posted this 17 February 2020

You don't have two elements through the thickness.

You have both Bonded Contact of the Bolt shaft to each hole, and you have Bolt Pretension, which can't work properly with the Bonded Contact. I suggest you delete Bolt Pretension.  If you do that, you don't need a 2 step solution and you don't need the nut.

If you decide to delete the Bonded Contact of the Bolt Shaft to each hole, then Under Analysis Settings, for Step 2, Auto Time Stepping should be On and the Initial Substeps set to 100. but if you delete the Bolt Pretension and have only Step 1, then use the same settings there.

You put 6 NR Residual plots under the Solution Information folder, did you look at them?  With one element you can see where the problem is. Remesh with 2 elements through the thickness. Set the Mesh to use Quadratic elements since you have long curved faces, you don't want flat facets on linear elements. It would be better if you can make fewer elements along the length and width while maintaining the 2 elements through the thickness. That way there are fewer nodes in the contact definition that have to resolve contact.

  

You might benefit from changing the Frictional Contact Normal Stiffness Factor to 0.01 but after it solves, check if the penetration is acceptable. All three frictional contacts can have the Update Stiffness set to Each Iteration.

Insert a Contact Tool under the Connections folder and check initial contact status. One contact is Near Open.

On that contact, change it to Adjust to Touch. You can do that to the other two also as it will help the solver to start.

I also recommended that you use a Displacement input instead of a force input. That will also make it easier for the solver to converge. You can put a remote displacement on the head of the bolt and push in the Y direction, you then request a Force Reaction on this Remote Displacement. I tried -50 mm.

Another suggestion with the Bolt Preload deleted and the Remote Displacement, it can be helpful to still have a 2 step solution. In step 1, the remote displacement is set to 0. That is just to let the contact resolve itself,  then in step 2, the head starts moving in -Y.

A final suggestion is to insert a Command into your model, NEQIT,50
This command will tell the solver to keep iterating for 50 attempts before bisection.  You can even tell it to use 100 iterations. The default is 26 iterations. Below is the Force Convergence graph for a 2 step model with adjust to touch and a -50 mm displacement. It is attempting 1% of that or 0.5 mm and it will need a lot of iterations for the contact to resolve because you have large surface area in contact. But look, it took more than 26 iterations, then gave a converged substep, we are off and running!

If it didn't converge with 50 (or 100) iterations, I would look at the NR Residual Force Plot and improve the element shape or reduce the element size in that area.

With two elements through the thickness, it will take a lot longer to solve, but if you cut it down to a 1/4 model as I suggested, it would solve 10 times faster.

If you convert this to a 2D plane stress model, it would solve 100 times faster.

Samyak97 posted this 17 February 2020

I tried remeshing with two elements on the thickness of the leaf. Meanwhile, the meshing on the upper face along the length got distorted and I could not correct it with any option in the mesh settings. Using the initial substeps brought back the solver pivot error and the errors:

"The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose."

"An internal solution magnitude limit was exceeded. (Node Number 58092, Body Unknown, DOF UX) Please check your Environment for inappropriate load values or insufficient supports.  You may select the offending object and/or geometry via RMB on this warning in the Messages window.  Please see the Troubleshooting section of the Help System for more information."

"Contact status has experienced an abrupt change.  Check results carefully for possible contact separation."

 

Sir, removing the bolt pretension does not make that much sense as the air gap or nipping of the spring is removed by tightening the bolt. The bolt provides the clamping force which hold the leaves together in the first place. 

It would be great if you could send the archive .wbpz file so that i could analyse how you did it.

 

I also made the contacts between hole of each leaf and shaft of the bolt as frictional instead of bonded.

peteroznewman posted this 17 February 2020

You are welcome to my file, unfortunately I started working on it in 2019 R3 so you won't be able to open it in 2019 R1.

I left it running and it had no problem, but I Interrupted the solution so I could plot some data. Here is the Force vs Displacement.

The spring rate is 99.5 N/mm.

Here is the starting shape and the point I stopped it at.

In my version, I kept the Bonded Contact to the bolt and suppressed the Bolt Preload.

The 348 iterations took 5 hours and 40 minutes on 12 cores.  Attached is an ANSYS 2019 R3 archive.

Attached Files

  • Liked by
  • Samyak97
Samyak97 posted this 21 February 2020

I am attaching a file, Sir. In the archive, please open the one named 'Quarter Model'. I am not getting any errors. And even the solving time is quite fast. But, the values are not desirable. So, please have a look and tell me where i am going wrong. I am guessing maybe the conditions I have set for the quarter model might be incorrect.  

peteroznewman posted this 22 February 2020

Did you upgrade to a newer version? I tried opening it with 2019 R1 and got an error message.

What is a desirable number?  Was the 99.5 N/mm spring rate I gave above desirable?

I replaced your force with a 50 mm displacement at the center.

I changed your Fixed Support on five faces at the center to a Displacement  Z = 0

I added a Displacement X = 0 to the five faces on the YZ plane.

I set the Initial Substeps to 100.

It did 709 iterations in 1 hour 50 min on 12 cores that was almost to 50 mm when I stopped it.

After I multiplied the Reaction Force by 4 to go from the quarter model to the full model, the spring rate was again 99.5 N/mm.

 

  • Liked by
  • Samyak97
Samyak97 posted this 22 February 2020

Sir, what is the total deformation and factor of safety you are getting with this model?

Can you please tell me how did you plot the Load vs Deflection /Force vs Displacement graph. Is the simulation not possible by using force instead of displacement? Please share your file. I will view it in a student version of R3 on another computer.

See i have done the simulation now in the "Quarter Model". But the only issue is that the factor of safety is coming out to be very less that is 0.088.

 Also, how to convert the quarter model values to full model?

Another doubt: If we try to realize the full model from the quarter model, how will it produce the result in the full model as the conditions are not the same on both the sides of the spring: one eye fixed and one eye with shackle. As the quarter model has shackle condition on the eye, wouldnt it consider the condition at the other eye as shackle(when full model is generated) instead of fixed?

Total Deformation:

 

FOS:

 

Force Convergence:

 

Equivalent Stress Von-Mises:

 

Max, Principle Stress:

 

 

I tried the simulation again and this time, I put the 50mm displacement on the top face of the bolt instead of the face of smallest leaf.

So, this time i got:

Still the minimum FOS is 0.18. The min. FOS should be 1 or something more than that. How do i get the proper FOS here?

Please Help.

 Is 50 mm displacement too much for the quarter model?

peteroznewman posted this 23 February 2020

Where is the minimum FOS?  Please turn on the Minimum flag on the results, then zoom in to that location.

If the minimum is at the bolt or bolt holes:

  • Turn off Bonded contact of the bolt shaft to the holes. That is not needed.
  • Change the Bonded contact of the bolt head to the small leaf to Frictional contact.

If the minimum is elsewhere, insert the image of that.

Samyak97 posted this 23 February 2020

Yes, the min was at the bolt or bolt holes. I suppressed  Bonded contact of the bolt shaft to the holes and changed the Bonded contact of the bolt head to the small leaf to Frictional contact. Still the min. FOS is 0.52 which is less.

peteroznewman posted this 23 February 2020

You can ignore the localized high stress under the bolt head because you caused it when you greatly simplified the real load path and artificially increased the stress by concentrating all the load through a small area. One way to more easily do the ignoring is to create a plane a short distance off the center plane. Slice all the spring leafs and use Shared Topology to reconnect them. Now when you do the Safety Factor plot, don't use all bodies, use the long end of the leafs and don't pick the bolt or the short piece around the bolt hole.

Another way to get rid of the localized high stress is to delete the Displacement BC on the bolt head and put the Force on the underside of the short leaf.  You can even slice the short leaf and create a short section near the center to apply the force over a much larger area than the bolt head.

If you don't want to ignore the localized high stress, then you must represent in a more realistic way that load path from an axle to the spring.

  • Liked by
  • Samyak97
Samyak97 posted this 24 February 2020

Ok sir. I wanted to ask about a mistake i made. For the quarter model, in the spaceclaim, i made two new planes and used the option of Split by plane in the Prepare section. Is there any way i can add the symmetry option (i did not find symmetry option in Spaceclaim, later found that its in DM) now in order to realize the full model results? 

Another doubt: If we try to realize the full model from the quarter model, how will it produce the result in the full model as the conditions are not the same on both the sides of the spring: one eye fixed and one eye with shackle. As the quarter model has shackle condition on the eye, wouldnt it consider the condition at the other eye as shackle(when full model is generated) instead of fixed?

peteroznewman posted this 24 February 2020

SpaceClaim doesn't automate the addition of Symmetry BCs after a Split by plane.  That is why I changed your Fixed Support on five faces at the center to a Displacement  Z = 0 and I added a Displacement X = 0 to the five faces on the YZ plane.  Those are the symmetry BCs.

Regarding one eye fixed and the other eye on a shackle, just change your point of view and you will see that the symmetry model can be equivalent if you leave the eye free along the Z direction.

Imagine attaching a camera to the axle that can see the spring flexing. Suppose the view of the camera is not quite wide enough to see the eye, but it can see almost out to the eye.  What it will see as the load is increased is that both ends of the spring flex downward equally. If all you saw was the view from that camera, you couldn't tell which eye was fixed to the frame and which eye had a shackle on it.

 

  • Liked by
  • Samyak97
Samyak97 posted this 25 February 2020

Sir, I plotted force reaction(Total) vs Total deformation(Max).

Is there any way so that the graph starts from the origin?

peteroznewman posted this 25 February 2020

Copy the tabular data and paste into Excel. Add a row and put 0, 0 in the first row. Plot the data in Excel.

  • Liked by
  • Samyak97
Samyak97 posted this 25 February 2020

I created  a quarter symmetric model using the symmetry option in DM. Then, used the exact same conditions i used before(The ones from which i got the above solutions and graphs). But,  I am getting error: "the solver engine was unable to converge on a solution for the nonlinear problem as constrainedPlease see the Troubleshooting section of the Help System for more information."  and the warning "The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose"

Show More Posts
Close