NL Static 3D - Bolt Connection with Preload

hooshsim

A blade and segment of a center disk are assembled using bolts connection as shown below. The objective to this analysis is to predict stresses around the blade holes.

A non-linear 3D static solution is obtained without any errors but Von mises stresses are missing due to non-converged solution. Per Victor's suggestion, I have added weak springs to eliminate the rigid body motion. This didn't solve the issue.

looking for recommendations on how to approach this problem? will adding bolt preload resolve the issue? If so, how do we apply it in Mecway/CCX?

I need to predict stresses around the blade holes.

Thank you in advance.

Sergio

Even if CCX solver has a specific PRELOAD card suited for this purposes, I'm still using the classical approach of adding thermal expansion coefficient to the bolt material and then apply a low temperature boundary condition to the bolt nodes to create the pretension stress. You need also to create a thermal stress boundary condition on Mecway to be able to use the temperature.

hooshsim

Sergio,
I’m not an expert in Mecway to add thermal expansion coefficient to the bolts. Do you have a sample or link on how to do this?
Thanks

Sergio

For the thermal expansion look in the material definition, is under the basic properties, young modulus and poisson. Then select the bolt component, change the selection mode to nodes and add a temperature below cero. Then go to the model tree and add a thermal stress boundary condition with a reference temperature

prop_design

Have you tried just fixing the bolt hole surfaces? I'm assuming you don't care about the bolt and nut stresses. To model bolt, nut, threads, takes a lot of elements and is usually done as a separate analysis. Just make sure to fix the actual surfaces that would be fixed. Usually the bolts go through holes and don't touch the cylindrical surfaces and only the washer locations are actually in contact. So I would try cutting the surface with the washer locations. That way when you bring the model into mecway you can select the washer surfaces in the cad area and fix them. This lets you try different meshes without having to reassign the boundary conditions. Also, I'm assuming you are using the CCX nonlinear solver. I have never had any issues with it not converging. Also, I'm curious why your blade seems at a weird angle to the bolt holes. Are you sure it's oriented correctly. It seems off axis to the the centrifugal load, so basically it looks like the whole blade is swept some. Perhaps you want that, not sure.

hooshsim

Sergio,
Just to make sure I understand your approach. First I should assign thermal expansion coefficient in the material properties for bolts only and then select the nodes on the bolts and assign temperature under New Loads and Constraints. Is this correct? Should I apply thermal concept to the bolts only or nuts as well?

prop_design,
I am interested in the stress values at the cylindrical surface of the blade holes. Fixing washer size surfaces on the blade flat surface will generate high localized stresses in the region...I will give it a try tho. And you're absolutely correct about the C.G. of the assembly being offset. It's only a generic model I created to show the problem.

Thanks and appreciate you both. Will give it a try.

Sergio

Will try to see the model later. What are the three components over the bolts and normal to them?

hooshsim

Those are weak springs suggested by Victor. Appreciate your support.

prop_design

oh i didn't see you attached the model. id love to try it as well. i model similar things. ansys workbench is really good for retention modelling, cyclic symmetry, bolt loads, and contact. but i got tired of a lot of its other issues and switched to mecway. it would make short work of this model though. there is a free version available. not the easiest program to learn how to use though.

prop_design

i took a look at your model. i attached a very simplified version. this is along the lines of what i was saying earlier of just fixing the washer faces. i wasn't sure of a lot of what you setup, so i removed a lot of things unrelated to what i was trying to show. this just gives an idea of how you could go about setting it up. you could add back in more of the features you had. i just wasn't sure what the design intent was. also, i couldn't figure out how to disable a part. it just seems to let you hide a component rather than disable it. all the cad geo wasn't present so perhaps the option to disable was there and i just didn't have access to it. so i just removed all the parts i didn't need.

also if you use cad to make the washer face cutouts in the surface you can get nice round surfaces to fix in the cad view of mecway. that makes it so you can remesh without having to redefine the boundary conditions. they will also be smooth too. doing it from the mesh makes them lumpy.

* updated in later post

prop_design

i'm wondering about your blade model. it seems like there should be fillets. the material says nylon. so i'm assuming this is a solid and not two plates welded together. but either way, looks like some fillets would be in order. i would also add a cutout in the area where the curved blade meets the flat blade. that way only the curved sides of the blade get filleted to the flat plate. this would make it so the fillets don't get really weird trying to wrap about the blade. so your model would basically have four independent fillets the way i am describing it. the bolts to the blade wouldn't touch the cylinders. there would be a gap between them as well. this is the normal way to bolt something together.

hooshsim

prop_design.

1. I am trying to model/analyze a bolt connect assembly to predict stresses around the blade holes. In your simplified version you have removed all the bolts/nuts and that's representative of my model. Can you suggest a solution to my original model with bolts and nots and contacts?

2. As I mentioned earlier, this is a generic model of the blade assembled to the center disk by virtue of bolts/nuts. The actual plastic part does have fillets and design properly.

Thank you again,

prop_design

ahh thanks for the clarification. sergio and victor will be better able to answer your contact quesiton. i used ansys workbench for a very long time and it excelled at that task. so going to mecway was so painful in that regards that i avoid doing that analysis type with mecway. there are so many things about ansys workbench that help to analyze what you want that it's too long of a list to state them all. i thought you were wanting the blade stress and not worried about the retention stress. in any event, before i got your post, i made an example with the fillet. it turned out the cutouts i was thinking of didn't work and you had to do a complete 3d fillet. so you get a little weirdness of two fillets coming to a sharp edge. but with the geo you have not sure how you would get around it. i make my blades and retentions completely different but we have some common issues. maybe the attached model will be of use to others trying to do something similar. also, notice how the deformation is consistent with the centrifugal force being aligned with the model. so the blade only twists and stretches. that's the best way to align it. i didn't apply the aero loads, since this was just trying to show the fillets and the blade alignment.

* updated in later post

prop_design

i played around with adding the bolt loads and cyclic symmetry. with mecway i usually can't use cyclic symmetry because it uses so much resources, whereas ansys does not. but in this example, i was able to get it to run. i have found in my tests and in this example that it really doesn't change anything much. with the preload i added and the cyclic symmetry the stress decreased slightly. so doing it the simple and fast way is slightly more conservative.

thinking on your model. i'm confused as to why you wouldn't be looking at the nylon part. the other parts were steel. so the blade is what would fail. the way i modeled it in the example should be loading the blade right. i don't think you need all the complicated bolts, hub, etc... but i may not be understanding what you are trying to do.

the free version of ansys is here; https://www.ansys.com/academic

there are a lot of products with it. i always used the workbench environment and it has a lot of great things. but a lot of frustrating things too. so that is why i switched to mecway. if you never used it, it may be too difficult to figure out how to use. if you know how to use it, it's very easy and fast to do most things. other things impossible. mecway makes a lot of those impossible things very easy. for me, mecway was a better choice as i only need to look at the blades and not the retentions. for retentions ansys workbench is a lot better. i have to be honest. even though it's a mecway forum. sorry

here are some comparisons with a bolt preload force and cyclic symmetry. if i tried to apply the preload moment it errored out.

i'm also attaching the updated model but i cleared the solutions to shrink the file size. configurations 1 and 3 are the most significant. four would be ideal but won't run. two was a test.

* updated in later post

hooshsim

prop_deisgn,
How did you add fillets to the model? Did you FreeCad software?
Thanks

prop_design

i have been using rhino 5 but have grown to hate it. i am waiting for moi v4 to come out. but if you are in a pinch you can use the moi v4 beta now and no charge to get v4 when it comes out. i was just waiting to save installation hassle. you could use rhino or moi. those are what i recommend for blade shape type stuff. i can do cars in them too. but a lot of people use poly modelers for that. it makes smoother blends. i don't care about the blends in my car models though. since they are just to get a basic idea of what is intended. but moi is very good. you can do a lot with it. and michael, the developer of moi is awesome, just like victor. moi is very affordable, just like mecway. so to me moi and mecway make a great team. you can do a ton of stuff with them often times better than super expensive software. but other times you may need something like ansys etc... i honestly think for your model, you can use the simple method i showed. but maybe i don't understand.

moi is here; http://moi3d.com/

prop_design

hi hooshsim,

i updated the cad model fillets. i was able to get rid of the sharp point in my first model. this is much better from a safety and manufacturing point of view. everything about the mecway model is the same. i just updated the geometry and mesh and re-solved. all the pics are for the updated model. i attached the updated model as well. hope this helps. i believe it addresses the stress in the nylon blade holes, like you wanted.

i cleared the results to save file size. just re-solve each config. config 1 is what i would do if it was me. config 3 is more like what you are going for. config 4 would be ideal but errors out. config 2 was a test i did.

anthony

prop_design

this is a pretty cool pic of displacement from config 3

prop_design

i experimented with the simplest bolted assembly i can think of. i don't see the value in trying to add this to your model. i will start a new thread with the example there. i have some questions and need others input. it's definitely a lot faster, easier, and more confidence inspiring doing it with ansys. with mecway it seems you have to make guesses as to various contact inputs. so no real way to know what the inputs need to be for the contact. i ended up setting them to the modulus of elasticity for the material i used.

hooshsim

Thank you, prop_design. I will look into it tomorrow.

prop_design

hi hooshsim,

ok i think i got what you want. i modified your contact setup based on the experiments i did with a test model. i can't say for sure if it's right as i'm not a mecway expert. but it converges and looks pretty cool.

* updated model in a later post

prop_design

* updated model in a later post

Victor

This solution uses bonded contact instead of contact so it's not really the same problem. Lateral loads on the bolts will be distributed around the entire circumference of the hole instead of only on the side that the bolt presses against. So the stress at the hole would be very different and it's not really correct.

I've struggled with this problem and can't work out why it won't work with only contact (no fixed supports or bonded contacts holding the bolts onto the plates). Some things I tried that failed:

• Moving one misaligned bolt back to the center of its hole.
  
• Adding bonded contact between the nut and bolt. (I also removed it between nut and plate, along with the fixed support there).
  
• Refining the mesh on the shanks and holes.
  
• Adding friction between the shanks and holes.
  
• Reducing the diameter of the bolts to ensure some clearance.
  

These things did help but likely aren't satisfactory:

• Changing from quadratic to linear elements.
  
• Ramping the loads - that succeeded with very small loads 1/100 of the original.
  
• Higher stiffness weak springs - leads to them carrying a significant part of the load.
  
• Bonded contact connecting the bolt to the hole.
  
• Reducing contact stiffness per unit area by a factor of 1000. I'm still waiting for it to solve but expect unrealistic penetration.
  

I'm a bit wondering about the suitability of a single FEA model for this problem though. The bolts seem to be loose which makes me think the stress could be sensitive to the size of the clearances between the various surfaces.

hooshsim

prop_design,

Great job. Your latest approach is more realistic than ones suggested earlier and the results seem to make sense as well. Great work!

Hooshsim

prop_design

i wouldn't say my suggested approach was not realistic. but it wasn't what you wanted apparently. honestly, i'm not sure what you want. the second time i just tried to get it to solve. it seemed like you didn't care about the bolt stress because the bolts weren't detailed. i just guessed that maybe you were just trying to connect dissimilar materials using contact. but in the bolt assembly example i posted in the other thread you can see how to analyze those if you wanted. it adds a lot of elements to the model. so it's not something i would do. usually you design the bolts with standard bolt calculations and leave them out of the fea model. in this model as i said i would just cut the surface where the washers go and apply forces and moments to them. one washer has torque applied in the positive direction the other in the negative directions. both washers get a compressive force applied. this way you don't need extra parts and contact.

prop_design

hooshsim,

i was starting to add more detailed BCs to the bolts and noticed your fixed BC was not right. you had some of the blot/nut faces fixed. this greatly changes the results since the cg of the assembly is off axis. i will post and update soon. i also have some added configs with extra layers of detail to the BCs

prop_design

hi hooshsim,

i attached an updated model. there are additional configurations. i noticed your fixed support didn't seem right. i tried to correct it the best i could. however, there doesn't seem to be geometry showing what fixes it in the z axis. in config three i selected some faces in that regard. but i would cut the surface wherever it is fixed in z so you can select it. instead of fixing the hole in all directions i would set the displacement to zero for xy. it can't be fixed in z from the inside of the hole as it is now. since the cg is off axis from the xy plane there is a substantial amount of stress and displacement compared to how you had it fixed.

i added some forces and moments to the bolts. they show what i would do but i don't know the magnitudes for the size bolts. you would have to do some calcs to find those out. i tried various values to keep the stress within reason.

so something along the lines of config 3 is where i would start. i would work on the fixed restraint like i said. i would also fillet the blade and the bolt if it were me.

you will probably have to experiment with the stiffness of the contact inputs. if you use ansys or something similar you will probably get better results.

but that's about the best i can do with it. the attached model has the results cleared to save file size. just re-solve each config. the first two solve in six iterations. the third config takes seven.

prop_design

hi hooshsim,

here is an update with perhaps better BCs. i noticed you didn't have the shank bonded to the nut. so i added that. i also changed how the forces and moments are applied. i changed the contact stiffness values. i changed the fixed displacement conditions. i experimented with the contact. what is attached is the best i can come up with.

as i mentioned before the shank shouldn't be in contact with your cd plate or the blade plate. it won't run unless i bond them. i would make the diameter of the two plates slightly bigger than the shank. it looks like you have a m10 bolt. so if you look for the fillet radius of that bolt, that is what the plate holes should align to. i used the min force and moment for the m10 bolt in config two.

i realized that the cd plate is moving a lot and the bolts are dense. i was thinking of a typical propeller where the retention is very stiff and only the blade is moving. in your model you do need the bolts in there for the density aspect. i don't know if you wanted the preload effect from the bolts. so i was trying to add that in case you did. this time i moved the force and moments to the plates figuring you weren't interested in the bolts. if you want to have the bolts accurate you would have to do a bit different setup. i have been working on it in mecway for an example bolt and it's a nightmare. so i would definitely recommend something better at contact if you want to get into the bolt aspect more.

just re-solve the attached model. i don't have the geometry files so i had to apply the loads and restraints to the mesh faces. you can do this better since you have the geometry files. i'm not sure what is restraining it in z so i just guess at that.

Sergio

Hi, this is how I would solve the problem, first using bonded contact for all, and in the case of trying to analyze more in deep the bolt behavieur I would add contact only in the blade to cd faces (still I would assume that during the normal use bolt/nut faces will be always in contact, so bonded would be still enough in that areas).


In this cases I like to work with multiple steps, first for bolt preloading and the second for the main loading (centrifugal acceleration in this case). As in Mecway that possibility doesn´t exist, what I did was change the time to 2, and use time 0 to 1 for bolt preloading and 1 to 2 for main loading, getting the same results using tables for loadings.
I include a thermal restrain in the bolts to create the pretension (70-85% of the bolt yield stress), and then the centrifugal acceleration. Have to add manually the cyclic simmetric boundary condition. For the blade acceleration have used 900 RPMs (would be nice to have RPM in the GUI directly).

In the X-Y plots what we see is the stress in the bolt shank, about 700 MPa for an 10.9 bolt. With more time what I do is divide the flanks of the bolt to apply restrain only in that portion and not in the head or thread that should not deform, but still in my humild opinion results are enough accurate for the matter.

hooshsim

Sergio,
This is great work. Thank you!
I resolved the convergence issue by Replacing “contact” to “bonded contact” for bolt head in my original model.
Thanks to all for sharing and contributing your support, specially Victor.