Connectors 'Bolt' Tool - Difficulties in selecting curved bearing surface/edge

[NatAmelbaines91]

Hi,

I seem to be having difficulties with using the 'Connectors' tool, in particular 'Bolt'.

I'm trying to carry out a very simple analysis where a clamp is being secured to a tube, at a fastening torque of 50Nm. Please see Screenshot 1. I think the issue lies with the type of bolt  'T-bolt' and washer used for this application.

I've practised using the Bolt and Connectors tool on flat surfaces and had no trouble but unfortunately the geometry of this clamp is curved and when selecting the bearing surface/edge for bolt head/nut it doesn't seem to register as a surface. Please see Screenshot 2.

I'm going to assume it cannot be done at a 'part' level but if there is any advice on how to get around this it would be much appreciated.

If required, I have the STEP file that I am happy to share. 

Thank you

Running Nastran In-CAD 2018

[John_Holtz]

Hi @NatAmelbaines91 

You are on the right track that the selected surface or edge for the bolt connector must be flat. The curved "saddle" shape of the hole going through the clamp will not work. In particular, the surface must be a flat, full annular area, or the edge must be a flat, full circle. See Bolt connector is not created in Nastran In-CAD for some examples.

It would be easier for you (but more difficult for the analysis) if you include the "washer" in the model. I assume the washer has a circular hole that could be used to define the bolt connector. You would then define separation contact between the washer and the clamp.

The alternative is more difficult to create (but easier for the analysis since it avoids separation contact). You could create a sketch in the part (in the Inventor modeling environment) that will become the shank of the bolt. In In-CAD (or Inventor Nastran, depending on the version), create a rigid connector using the edge of the hole (the same edge that you are selecting to try to create the bolt) and the end of the bolt. Create a new idealization, and create beam elements using the sketch line. Enter the preload for the beam elements on the Idealization dialog. (Note that I have not tested the rigid connector, but I think it should be able to use the saddle-shaped edge. The rigid connector should not be limited to flat edges.)

[NatAmelbaines91]

Thank you John. I will try both of your recommendations.

[NatAmelbaines91]

Including the washer and manually defining the separation contact between the clamp and the washer appeared to work out ok (please see screenshot attached). For the connector loading, a torque of 50,000 N.mm and a torque co-efficient of 0.25 was applied.

FYI - Unfortunately, the alternative method of applying the rigid connector didn't appear to work for me. I was unable to select the saddle shaped edge (screenshot also attached).

[John_Holtz]

Hi @NatAmelbaines91 

For the rigid connector, you did not select a point for the "Independent Vertex/Point > Select Point". You need to highlight the box (so that it is blue and ready to select a point), and then select the end of the beam/sketch. This will connect all of the nodes around the saddle edge to the end of the beam; that is, make a "head" or "nut" for the bolt.

[NatAmelbaines91]

Hi @John_Holtz ,

I have re-attempted using the guidance you have provided. Thank you for that.

I've obtained a solution but the stress result appears to be much less when compared to the analysis where I have used the washer. I think somewhere along the lines I have made an error. I have attached some screenshots that show my approach to using this method.

Also,when double checking the initial simulation (using the washer) using the 'animate' feature. The simulation doesn't appear to be correct. This is due to the 'fixed' constraint I have applied to the inside spherical faces of the clamp. Are you able to advise a suitable constraint that will enable me to analyse the whole clamp as a result of the bolt preload? I did read the following link: https://knowledge.autodesk.com/support/nastran-cad/learn-explore/caas/CloudHelp/cloudhelp/2019/ENU/N.... But I do not appear to have constraint types:  'frictionless' or 'pin' as quoted in the link.

My next simulation will be to simulate a tube being clamped by the clamp (no doubt I will have more questions regarding this) but I wanted to make sure that I at least get the simulation correct for the clamp in isolation.

Thanks again.

[John_Holtz · Accepted solution]

Hi @NatAmelbaines91 

It looks like you have one rigid connector that connects the "head" and "nut" end of the clamp to one end of the beam/bolt.

You need two rigid connectors:

1. The first rigid connector for the head of the bolt, connecting the circle on the clamp to the head end of the beam/bolt.
2. The second rigid connector for the nut of the bolt, connecting the circle on the other side of the clamp to the nut end of the beam/bolt.

Regarding the analysis with the washers, pin constraints were added in version 2019.1, and frictionless constraints were added in version 2019.2. They are not available in your 2018 version. What you can do is create a cylindrical coordinate system and apply a constraint to the inside of the clamp so that the nodes cannot move in the radial direction, but are free in the hoop direction. This article describes how to create a cylindrical coordinate system and apply the constraints in the coordinate system: How to represent 2D axisymmetric elements in Nastran In-CAD. Instead of applying a symmetry constraint as described in the article, you will be applying a Tr constraint to fix the radial displacement.

[NatAmelbaines91]

Thank you.

I have re-attempted based on the recent information given. I now seem to get similar results to the analysis that includes the washer. The reduction in computational time is a bonus too. Screenshots are attached, should you wish to review. (Any comments/concerns are much appreciated).

Fortunately I have Inventor 2020 on my own personal laptop and have access to the 'frictionless' support constraint (2018 is the version used by my employer). I'm still having difficulty with that when analysing the tube but I will create a new separate forum post regarding this.

Thanks

[felixjr11]

@John_Holtz,

Sorry to open up this topic again, if you remember me I'm new in Inventor Nastran.

Can I used this procedure to simulate bolted connection in a shell element? if not what is better solution.

I have this 2 panel that I want to know the stresses in bolt, and plate connection. I'm more interested if the they can withstand the concrete pressure.

Kind regards

Felix 

[John_Holtz]

Hi @felixjr11 

I'm not sure what part of "this procedure" you are referring to, so let me ask some questions and provide some general comments.

1. You can use a bolt connector. 
2. If the bolt connector does not work (why not?), you can draw a sketch and create beam elements for the body of the bolt, and then use two rigid connectors for the head and nut/thread.
3. What does "concrete pressure" mean? Where does that come into the analysis?
4. What element types are you using? I cannot tell from the image if you have a surface model or a really thin solid model.