Learning Forum

[GopinathV]

I have done a static structural analysis of an assembled component that uses bolt connections and welds. I had defined two type of loads, 1.Bolt pretension 2.External load as force.

I have defined bonded contacts for all the bolt, nut interfaces and the surfaces that were mated for assembly. The results were not as expected. I got a peak von mises stress of 960MPa, near the bolt hole region, whereas the ultimate strength of my material (structural steel in ansys) is only 460MPa.

NOTE-1: I have previously defined frictional contacts for bolt head and nut head interfaces, but it resulted in DOF limit exceed error and newton raphson residual showed  my elements flew off in space. So i switched all my contacts to bonded type and got this undesired result. I am sure the component wont fail (from the experiments) that is it can never develop this high stress value. 

NOTE-2: I have redesigned my original component with a generic model and have used it for this post

Please direct me to find where the problem is in this analysis, i have attached with this the post my archived workbench file

[peteroznewman]

Hello Gopinath,

You will get much better results using Frictional Contact under the heads and nuts than Bonded Contact, but you have to check that the contacts are closed. Put a Contact Tool under the Connections folder and Generate Initial Contact Status. If any contact is not closed, you have to take corrective action such as setting Adjust to Touch on that contact.  You also turn on Auto Time Stepping and set the Initial Substeps to a large number like 100 to give the solver a chance to establish contact before too much bolt pretension has occurred. That will prevent the Exceeded DOF Limit error you are seeing with the parts flying out into space.

Then you have to wait longer for the solution for Frictional Contact because the solver has to iterate to find the contact and it doesn't have to iterate for a Bonded Contact.

To reduce the node count in the mesh you should learn to take advantage of symmetry. The load and geometry are almost symmetric. I expect you can ignore that the base plate is wider on one side than the other. Do some geometry simplification. Delete all the small blends on the part with the cylinder except for those on interior corners. Delete all the blends off the screw and nut heads. You are adding a lot of nodes to the model for very little benefit. It will solve faster is there are fewer nodes.

 

After making those changes, the mesh reduces from 1.8 million nodes to 0.6 million nodes.

 

Regards, Peter

[GopinathV]

Thank you Peter...i shall work on the geometry simplification part. Although i would find the frictional contact definition quite challenging . i had an instinct that my contact definition is what kept causing me too much troubles, but if frictional contacts definition is the correct methodology to constrain my model then i shall work my way into that. i shall update this after i try again with frictional contacts.Thanks again

[GopinathV]

And your suggestion about the symmetry of the model, did you mean to suggest me to slice up my whole assembly along the XY plane into half?

[peteroznewman]

Yes, down the center of the main bracket.

Updating Bonded Contact to Frictional Contact is as simple as selecting all the bonded contacts in the Outline, and using the pulldown where it says Bonded and picking Frictional and entering a COF.

 

 

[GopinathV]

It dint strike my mind at first, but i am surprised when u did remove those blends off the fasteners and pin, and remeshed it. May i know how u did that?

[peteroznewman]

To delete a face in SpaceClaim, click the face and hit the delete key. If it can, SC will trim the adjacent faces to close the gap.

[GopinathV]

Good to know about this. Thank you peter. 

One other thing, i shall define frictional contact between surfaces of bolt head and nut head with its components in contact, but do i define all other surfaces in contact to be bonded? For example, the cylindrical pin and the bracket are not supposed to be separated after they are being fastened by bolts, so the surface between pin and bracket should be defined a bonded contact and all other surfaces that have been mated during assembly of components should also be defined bonded contacts. Am i right here?

[peteroznewman]

The only bonded contact would be nut to bolt, except for the bolts that go into the bracket where there is no nut, those could be bonded. There is an alternate approach that simulates threads, but that might be a topic for another post. 

All the faces being clamped together by the nuts and bolt heads should be frictional contact.

[GopinathV]

OK thank you again.

I have also modeled weld between bracket's side edge and support plate. What type of contact would they have between their surfaces?

I never thought the contacts in the analysis would be this difficult and important!

[peteroznewman]

Yes, bonded contact is appropriate for each weld face to the mating part. I forgot about those!

[GopinathV]

Thanks once again. I shall update this post if i find trouble establishing initial contact with frictional contacts

[GopinathV]

Peter, after implementing your suggestions on frictional contacts and giving sufficient substeps for loads steps, mu solution converged. Yet, i still have peak stress values around the bolt holes to be exceeding the uts value.
one important thing to be noted is that my total deformation doesn't exceed 0.2mm while the von mises stress is around 700MPa.
Can someone explain what could possibly have gone wrong?

[peteroznewman]

Which holes have the high stress? Are you sure it is the hole and not the bolt head. You can ignore high stress under the bolt head where you left a sharp interior corner as the real bolts have a small radius that limits the peak stress.

If it is the through holes, you should confirm that there is no dependence of the result on element size by reducing the element edge length by a factor of 2 around that hole edge and the bolt head that has frictional contact with the face.

If it is the threaded holes, you can change from bonded contact to frictional contact and add the Geometric Modification of Bolt Thread to the contact definition and use mesh controls to have element size no larger than 1/4 of the pitch on those faces.

If the true solution is that the stress exceeds UTS and you don't want that, then you have to redesign the assembly and use more bolts.

If the true solution is that the stress exceeds the UTS and you want to see the plastic deformation, then add plasticity to the material model and let the material stretch after it reaches its Yield Strength. The simplest plasticity material model is Bilinear Isotropic Hardening. Enter the Yield Strength and type 0 for the Tangent Modulus. This defines an Elastic Perfectly Plastic material.

[GopinathV]

Peter, to answer your first question, the through holes have these high stress values and not the threaded holes.
As for the second question, yes i am sure the holes does experience high stress and not the bolt head. Rather an even more peak stress of 900MPa occurred on a circular edge of bolt shank face where i had split a face along the lengh of bolt to differentiate the shank face (to define pretension load) and threaded part (modelled as smooth cylindrical surfaces)...i shall, however, try on the mesh dependence and i am also sure that plastic deformation cannot happen

[peteroznewman]

• What preload are you using? 


• What is the fastener size and grade of material? 


• What is the torque spec you specify for tightening that fastener?

You could add a washer to the design to spread the load over a larger area.

[GopinathV]

I had used M20, M16 and M14 bolts of grade 10.9. Material selection ISO R898..i created the engineering data for that material from a data sheet..other than isotropic coefficients, density and strength values i had also defined bilinear isotropic hardening properties with yield strength and 3% of young's modulus as tangent modulus. All preload values were defined according to specified values of pre-torque for metric bolts. Preload values are: M20 - 125kN; M16 - 96.87kN; M14 - 71.43kN.

Also i have attached a screenshot showing the peak stress value of around 700MPa and exactly where it does occur on the bolt hole region (of the front face of bracket), for reference

[peteroznewman]

It looks like you are showing a hole that in the real part would be tapped and have threads, but in the model has bonded contact. Am I right?

If it is the threaded holes, you can change from bonded contact to frictional contact and add the Geometric Modification of Bolt Thread to the contact definition and use mesh controls to have element size no larger than 1/4 of the pitch on those faces.

[GopinathV]

oh ok peter, i knew about bolt section method previously. but i thought creating a MPC bonded contact instead would reduce my computation time.
And yes i will try that option now.
But one question though; i had used a M20 bolt in the design and had defined 125kN of preload...how high value of stress is expected out of pretension bolt loads?

[GopinathV]

And regarding the bilinear isotropic hardening, i should define the materials yield strength value and tangent modulus be assigned zero right? if that is the case, should i turn on large deflection in the analysis settings?

[peteroznewman]

Yes, MPC bonded contact reduces computation time and is a less accurate method of representing a threaded fastener connection.

Using linear materials reduces computation time and is a less accurate method of representing stress in the model that exceed yield strength.

If you have checked that you have a sufficient length of thread engagement to avoid stripping the threads when applying the correct preload, then you are done. You could make an element selection that selects all the elements in that part except for the elements on the face of that hole. That is one way of ignoring elements you don't care about because you have a good reason to ignore them.

If you change the material of that part to a bilinear isotropic hardening plasticity model with zero tangent modulus, you won't have any stress above yield strength anymore (except for extrapolation to the nodes, see ERESX command). Whenever you turn on plasticity, you should also turn on Large Deflection.

You could also change the contact to Bolt Thread geometry and put a lot more elements on the hole face. You might still exceed the UTS with a linear material, in which case, you can use the nonlinear material.

[GopinathV]

I did use linear material (structural steel) primarily because the assembly was tested experimentally for fatigue failure and it ran without any failure or cracks for 2 lakhs cycles.

So, my simulation is expected to have maximum stress anywhere in the bracket to be lesser than the yield value, which i ma not able to simulate properly because the bolt pretension caused too much compressive stress. 

Hope i have given a clear idea of my simulation now.

NOTE: Still couldn't figure out why bolt pretension causes extremely high stress values.

[GopinathV]

I finally modelled with frictional contacts between all surfaces between nut and bolt and bonded MPC for thread geometry, switched to nonlinear material selection with BISO properties defined and turned ON large deformation and i was able to simulate it correctly.
Thank you peter

[Simo]

I finally modelled with frictional contacts between all surfaces between nut and bolt and bonded MPC for thread geometry, switched to nonlinear material selection with BISO properties defined and turned ON large deformation and i was able to simulate it correctly. Thank you peter

Hi GopinathV,

I have your same problem.

I want ask you if is it possible to attach your final model, just to let me know how is it possible to solve my problem.

I have no idea hot to set non linearity on my model.

Thank's in advance for helping me

Simo

[GopinathV]

Hello Simo

Firstly, you can have a look at my final model that i have attached as an archive file with this post.

Secondly, regarding non linearity i guess you might have referred a few other posts and would have learned that there are three types of non linearities in an analysis. Geometric non linearity; material non linearity; contact non linearity. So i need clarity on which type of non linearity you are dealing. 

Suggestions on non linearity in ansys:

1. For  material non linearity the simplest method is to define bilinear isotropic hardening properties (in engineering data) by entering a material's yield strength and tangent modulus. And then assign this material to the part/ component you have modelled and make sure right below the non linear material effects are turned ON

2. For geometric non linearity, simply turn ON "Large Deflection' under solver controls in Analysis settings, when you are not sure your analysis would involve  large deformations

3. For contact non linearity, check if you are dealing with frictional, frictionless or rough contacts

 

[Simo]

Hi GopinathV,

thank's for your answer.

I was referring to non linear behaviour of material, so I've just defined isotropic hardening properties.

I have Ansys workbench student version, and to semplify my model I've set for all bodies your same material EN8 Steel.

I am able to run my analysis but I don't like results, since around the 4 holes on the bottomer plate, I have stress concentration around the edge.

I haven't applied any load (pressure is suppressed), only screw preload.

Thank's again for your helping

Simo

[Simo]

Hello Simo

Firstly, you can have a look at my final model that i have attached as an archive file with this post.

Secondly, regarding non linearity i guess you might have referred a few other posts and would have learned that there are three types of non linearities in an analysis. Geometric non linearity; material non linearity; contact non linearity. So i need clarity on which type of non linearity you are dealing. 

Suggestions on non linearity in ansys:

1. For  material non linearity the simplest method is to define bilinear isotropic hardening properties (in engineering data) by entering a material's yield strength and tangent modulus. And then assign this material to the part/ component you have modelled and make sure right below the non linear material effects are turned ON

2. For geometric non linearity, simply turn ON "Large Deflection' under solver controls in Analysis settings, when you are not sure your analysis would involve  large deformations

3. For contact non linearity, check if you are dealing with frictional, frictionless or rough contacts

 

I am not able to run your model since student version has some limits on the number of nodes

[Simo]

I think I've solved my problem...I obtain a regular stress distribution around my holes.

But I have some doubts.

1- Auto time stepping in Analysis settings : what does this funcion make?

2- Newton-Raphson residual: what does this function represent?

Thank's again

Simo

[GopinathV]

1. Auto time stepping is set by the solver for optimised time increments through which load applied will gradually increase so that the resultant non linear response will be better captured. Load can also be increased by manually giving time step size. smaller the time step size smaller will be the load incremented value

2. Newton raphson residual tells you how deviant your solution is from the exact solution. In ansys the erroraenous result caused due to non convergence or rigid body motion can be plot using the newton raphson residual by adding a newton raphson residual option under solution tree

[patilyogesh.a9]

While applying bolt pretension, why we have to lock load in next load step?