## General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

#### Bolted joints modeling for MoS calculation

• Gianluca De Zanet
Subscriber

Hello,

I am starting to model bolted joints in my assembly, and I am not fully conviced which is the more convenient way to do that. The goal is to calculate the Margins of Safety (MoS), so that I would need an model from which I can extract three forces and three moments.

I remember that bolts can be modeled in MSC Nastran by connecting the centres of the holes and the rest of the structure with RBE2 elements, and then by connecting the centres of the holes with CBUSH elements. I am not sure if preload could be modeled this way though. My question is: is there a similar approach in Ansys?

Many thanks,

Gianluca

• Nanda Veralla
Ansys Employee

Hello Gianluca,

I'm not sure about the workflow of Nastran, because I've never used that. But if connecting parts by bolts, and you're looking to efficient ways in doing this, I highly recommend this Ansys Innovation Course on modelling bolt connections:

Connecting Bolts with the Rest of an Assembly | Ansys Courses

After course completion, you'll be familiar with connecting bolts as solid and line bodies. Let us know if doesn't help your case.

Regards,

Nanda.

If you are not able to open the links, refer to this forum discussion: How to access the ANSYS Online Help

For more exciting courses and certifications, hit this link: Ansys Innovation Courses | Ansys Innovation Space

Guidelines for Posting on Ansys Learning Forum

• Gianluca De Zanet
Subscriber

Hello Nanda,

The thing is that for the MoS calculations I would need certain quantities (namely Axial Force, Shear Force, and Bending Moment) that I cannot get from the beam probe. However, I have just found out that I can request those quantities as User Defined Result, so that now I think I can retrieve what I want.

Does it make sense?

• Nanda Veralla
Ansys Employee

Hello Gianluca,

Yes, you are correct. You can retrieve them by using user defined results.

In case you are unaware, Ansys has another feature called "bolt thread contact" which models a simple cylindrical face into threads numerically. This feature is available under contacts-->geometry modification. This might be the best approach for calculating MoS calculations accurately.

Geometric Modification (ansys.com)

3.8. Geometry Correction for Contact and Target Surfaces (ansys.com)

• Gianluca De Zanet
Subscriber

Ok, thanks for confirming that. One further question about the modelisation with bushings to reproduce the approach in Nastran: am I wrong or it is not possible to associate any pretension element to the bushing?

• Nanda Veralla
Ansys Employee

Hello Gianluca,

I’m not aware of how Nastran models bushings, but from Ansys point of view, pretension can be applied for solids, line bodies or beam connections. I’m leaving this comment, to ask you to reply back with screnshots of your workflow and detailed description. Probably someone, who’s familiar with both Ansys and Nastran will guide you further.

Thanks,

Nanda

• peteroznewman
Subscriber

I am familiar with both Ansys and Nastran.  In Nastran, I have used the CBUSH element to connect two coincident independent nodes of two RBE2 elements that spider out to the edges or faces of the holes.

To do the same thing with Ansys, you can create a Joint, type = General and scope the mobile side to one hole and the reference side to the other hole. If you set the Behavior to Rigid, that is like an RBE2 element, if you set the Behavior to Deformable, that is like a Nastran RBE3 element.

https://forum.ansys.com/forums/topic/how-to-replace-connector-elements-available-in-abaqus-with-6-dof-spring-in-ansys/

You can't define a preload using the above method, but there are other ways to create a preload in Nastran and Ansys.

• Gianluca De Zanet
Subscriber

What is very interesting to me is that the application of this kind of joints seems very rare in Ansys, and approaches with line bodies or beam connections are preferred. I have received a feedback on beam connections, and I will try to summarise for confirmation. The steps are the following:

1. Imprint head/nut bearing area on mating surfaces
2. Create remote points with MPC formulation and rigid behaviour attached to the bearing areas
3. Connect the remote points with beams
4. Probe the results by simply using a beam probe.

As far as I understand, this approach Is recommended when compared to simply connecting the bearing areas with beams. One question: in the case of threaded hole joints, is it correct to define the second remote point by selecting the cylindrical face of the thread, and then connect it to the beam?

Yesterday I have noticed that I can retrieve the quantities I need also by defining some User Defined Results; however, it seems to me that all the quantities obtained with the beam probe are actually those I am looking for. More specifically, the shear forces at nodes I and J represent BEAM_SHEAR_FSUM, and for some reason the moments at nodes I and J represent the maximum and minimum values of BEAM_BENDING_MSUM. Then, the maximum value of BEAM_BENDING_MSUM should be added as an additional component of the axial force BEAM_AXIAL_FX for the MoS calculations.

The post-process should be automatized at some point, but that’s another story.

Does it make sense at all?

• peteroznewman
Subscriber

Hello Gianluca,

That is a good summary. Yes, for threaded holes, scope the remote point to the face of the threaded hole.

One advantage to using a Beam compared with a Joint is the ease of obtaining correct output. The beam has a line that defines the axial direction and the shear directions are correctly labeled. Forces in Joints are labeled with X, Y, Z coordinate directions, but you have to know which axis is axial and which axes are shear directions.

Another advantage to using a Beam compared with a Joint is that you can apply a Preload force, though you must also define a frictional contact between the faces being clamped together by the fastener.

One difference between a Beam connection (where the beam is automatically created) and a Line body meshed with beam elements is if you have a temperature load, CTE effects such as the beam getting longer or shorter with temperature changes will not be calculated on the Beam connection, but it will be calculated on the beam elements on a Line body.

A significant defect in Ansys compared to Nastran is in the behavior of the spider from the Remote Point to the scoped nodes on the face or edge of the part when a temperature load is applied. In Ansys, for Behavior = Rigid, there is no ability to define a CTE value for the spider. In Nastran, when creating an RBE2 element, you can define the CTE for the spider. This means that when the CTE is the same for the body and the RBE2 element, there can be a stress free thermal expansion of that connection in Nastran. In Ansys, Remote Points will create stress around the hole under a temperature load.

I hoped that changing the Remote Point to Behavior = Deformable would deliver a stress free result under a temperature load, but I was disappointed to see stress on the edge of the hole when I tried that.

The workaround in Ansys to avoid stress around the hole under a temperature load is to create the spider using beam elements meshed on line bodies, which is an unacceptable amount of work. It is less work to put a solid model of the fastener and use Bonded Contact for the bolt head and threads to obtain a stress free result under a temperature load when all the CTE values are equal.

• Gianluca De Zanet
Subscriber

For any thermal gradients affecting the bolted joints, I would say that their contribution for MoS calculations might be hand calculated for now. It seems to me that thermally induced forces affect the maximum and minimum preload in the fasteners, and that should depend only on the CTEs, Young's modulus and force ratio. Please correct me if I am wrong, and if I am missing something.

I do have another doubt, that perhaps needs to be addressed before the bolts analysis itself. How could I size the bolts correctly, i.e. how could I determine their workload and hence their diameter? I think I have read a post from you @peteroznewman in which you were saying to connect the parts with preliminary holes rigidly and then extract the forces? Could you please elaborate a bit about this?

• peteroznewman
Subscriber

One methodology uses the CBUSH element (or Fixed Joint) force output for Axial and Shear Force.

Those numbers are put into a Bolted Joint spreadsheet (or online calculator) to find the size of bolt that will carry the axial load without joint separation and that can support a bolt pretension load sufficient to prevent joint slippage due to the total shear force.  Of course the bolt pretension can only go so high before the bolt yields or the threads pull out. If this happens before the joint slippage is eliminated, then a larger bolt size is required.

The thermal CTE effects can be computed in the Bolted Joint spreadsheet if temperature limits are included in the inputs.

• Gianluca De Zanet
Subscriber

Thanks for your help, but I still don’t fully understand the set up of the Fixed Joint and the first steps to take.

Hence my questions:

1. Should the parts have already sort of “preliminary” holes, and the Fixed Joint defined between the cylindrical surfaces of these holes? Or the “preliminary” holes are not necessary for the Fixed Joint, which is then defined between the mating surfaces? The latter would make more sense if the goal of using the Fixed Joint is to determine the workload, which I suppose can be divided among N fasteners?
2. I expect that the Fixed Joint will replace the contact defined between the same surfaces, and only after the bolts size and number are determined, contact has to be reintroduced?
3. Which behaviour is recommended for the Fixed Joint in this case, rigid or deformable?

Thanks for confirming that thermal effects can be hand-calculated, this takes away many simulation issues!

• peteroznewman
Subscriber
1. If the design is so preliminary that the number and location of the fasteners is not yet fixed, then defining a joint between the mating surfaces seems like a good idea to decide on the total number and a rough initial sizing.
2. After the number and locations has been decided, add nominal holes at those locations and create a Fixed Joint at each hole pair. Some Joints will carry more load that others. Sort the loads to find the hole pair that has the highest axial force and the highest total shear force. Now you can use those numbers to make a final selection of the fastener size.
3. The force going through the Fixed Joints will not be significantly different between the rigid and deformable behaviors, so for bolt sizing you can use either one. However, if you also want stress output on the mating parts, the rigid behavior is more likely to create a stress concentration artifact compared with the deformable behavior.
• Gianluca De Zanet
Subscriber

I have received a feedback on the use of Fixed Joints for pre-calculations, and that confuses me a bit. It is suggested to establish only Fixed Joints between the interfacing parts, with no other contacts. Then, the joints have to be defined in the conic pression zone of each bolt in the interface (I presume imprinted area of the analytical calculated compression diameter?). Finally, the workload can be retrieved by using joint probes, and the bolts can be sized accordingly.

Is this a valid approach? It just seems that there is not an unambiguous way of doing that, and it would be great if that could be clarified.

• peteroznewman
Subscriber

Most nuts and bolt heads have a washer under them. If you imprint the washer diameter on the surfaces of the mating parts, that is a good place to start.

Some models have a large number of bolted connections. Ansys has a tool to rapidly create a large number of connections by using a combination of Named Selections, using the Size checkmark and the Object Generator to automatically make copies of a Fixed Joint over all the items in a named selection. Here is an old video that demonstrates this feature:

If the parts being joined are thick solids, when you create a Fixed Joint and select the Reference side of the joint, the centroid of that area is where the joint coordinate system is placed. This means that the spider from the area on the Mobile side of the joint will reach up through the two thick solids to get to the coordinate system. This is not ideal. The ideal is to place the joint coordinate system on the joint axis at the mating plane. You can edit the origin of the joint coordinate system after the joint is created. I have a trick when making a joint to land the coordinate system in the ideal location. Set the object filter to Edge instead of Face and pick an edge of a hole in the mating plane as the Reference side. This will locate the joint coordinate system in the mating plane. Then change the object filter to Face and pick the imprinted washer area for the Mobile side and then click the Reference side to replace the edge with the imprinted washer area for the Reference side. Now you have a Fixed Joint where each spider reaches down to the mating plane.

After analyzing the stress in this model full of Fixed Joints, you might find that one or more of the joints is in a highly stressed location. That is when you can consider building a detailed model of that bolted joint. Delete the Fixed Joint. Add a solid model of the nut and bolt (without threads) at those holes. The nut and bolt head can be modeled as cylinders at the washer diameter. Add Frictional Contact between the mating surfaces. Split the shank of the bolt cylindrical face at the plane of the nut. Add a Bolt Pretension load to the bolt shank face. Add Bonded Contact between the nut and bolt shank that is inside the nut. Add Bonded (easier) or Frictional Contact (more accurate) between the imprinted washer faces and the nut and bolt head. Now you have a very detailed model that will be far more accurate for stresses around the bolted joint than the Fixed Joint.

Frictional contact is nonlinear while the Fixed Joint is a linear model. This means you may have to do extra work to get the solution to converge such turning on Auto Time Stepping and setting the Initital Substeps to 10 or 100 to get the convergence started.