Hoisted load with cables - How to model?

[Anonymous]

Hello,

I am having some problems when modeling a structure consisting of a frame, that is being lifted by four cables, one on each ending of the frame, as seen on the image below. This frame has also vertical loads applied to it.

My first approach was defining a simple round section and defining it as a beam, representing my cable.

• Here I got to the first problem: I could not trust totally on the model, because I could not establish a "Beam End Release" to the beam elements representing the cables (I found an Autodesk help page about it but I simply couldn't follow it, I didn't find where the instructions indicated), which means my "cable" is transmitting moment to my frame.
• Also, when checking Buckling, I kept getting the smallest eigenvalues on the cable (of course being negative, because the cables are tractioned, not compressed). I wanted to skip the cable and only analyze the frame for buckling.

Then came my second approach: using a "Cable" connector as a substitute for the "beam" cable of the first approach.

Then, I got my third issue:

• If I define a "Cable" connector, the software doesn't seem to understand that the end of the connector is a valid point for inserting a constraint. I added a sketch point on it to be sure, but it doesn't work at all. Keep getting 5001.

All that being said, I ask:

• Am I modeling it correctly? Is there any better way to model this scenario (hoisted frame)?
• Could anyone give me a more detailed and visual instruction on how to add a Beam End Release?
• How to "skip" the first mode of buckling, and even get the second, third, etc? Or ignore specific regions if the model?
• How can I define a constraint to the end of a "Cable" connector?

Any help is appreciated!!

Best Regards,

Fadi

[John_Holtz · Accepted solution]

Hi @Anonymous 

The important thing that I see is you have applied constraints in the horizontal direction to make the model statically stable in those directions. I like it. 😊

Here are comments on your 4 questions.

1. Is it modeled correctly? See knowledge.autodesk.com > How to perform analysis of lifting frame in Nastran.
2. How to add a Beam End Release? See knowledge.autodesk.com > How to define beam end releases in Nastran In-CAD. (Nastran In-CAD is the former name for Inventor Nastran.)
3. How to "skip" the first mode of buckling? See knowlege.autodesk.com > How to interpret negative eigenvalue buckling results in Autodesk Nastran In-CAD.
4. How can I define a constraint to the end of a "Cable" connector?
   1. First, cable connectors are only applicable for nonlinear analyses. Are you performing a nonlinear analysis?
   2. If performing a linear analysis, you should use a Rod connector instead. (That will also eliminate question 2, but I am not sure if a rod element can be used in a buckling analysis.)
   3. I assume the beam elements for the cables were define using sketch lines. Is that correct? And the constraint at the top of the hoist is attached to the end of the sketch line. The rod and cable connectors are almost the same. Instead of selecting the sketch line, you select the two ends of the sketch line to define the two end of the rod or cable. Because the rod or cable and the constraint are using the same sketch point, the constraint is attached to the rod or cable.

The alternative to modeling the hoist with elements is to define 4 local coordinate systems with the Z axis aligned with each cable. Then apply a constraint with the local Z direction fixed.

[Anonymous]

Hey @John_Holtz!

Thank you for your kind reply!

1) I'm glad to see my model is compatible with the recommendations! Thank you for this link! Also, it helped me establish the correct conditions to set the constraint on the top of the hook (end of connectors). I couldn't get the constraint on the end because I didn't have any "free" sketch there. I created another part, with only a sketch (not the one used to create the connectors), put it in the assembly (It is an assembly because I used Frame Generator) and it worked!!

2) Yeah, I have found this link aiding on the Beam End Release matter. Honestly, I couldn't do it because I got stuck on this: "right-click on ELEMENTS and choose DISPLAY LINE ELEMENT > DIRECTION". I couldn't find where this ELEMENTS is. But, as you pointed out, I don't need this if I use Rod connections, which I did and worked (after your link sent on 1).

3) Worked like a charm, thank you so much for this.

4.1) Yes I am using non-linear analysis. After I put the constraints correctly it worked.

4.2) I also could run buckling analysis with rod connector, had no trouble with that.

4.3) I couldn't use the same sketch that I used to make the cable / rod / beam (tried the three), I don't know exactly why. This was my struggle. So I made another part with a new sketch, joined it on the assembly, positioned it correctly, and voilà.

I understood the alternative theoretically, but I have so much trouble with this UCS stuff. I prefer not to enter that terrain for now. But I will keep it in my "toolbox", this tip (rotating the constraint to a specific degree) seems useful.

Man, I can't Thank you enough.

Regards,

Fadi