Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

Beams no moment

Good morning!

I'm trying to model the 4 cables shown in the attached file. At first I thought of using Beams to make it easier but the fact is that those cables cannot transmit moment (rotation) in the joints (2 joints in each cable). How should I do it? Do I change the element type? Is there any way of erasing restriction of the rotational DOF at the joints?

Hoping a quick response and thanks in advance!

Unable to find an attachment - read this blog

Find more posts tagged with

English

HyperMesh

Accepted answers

All comments

tinh

Use CBEAM (1d>bar2)

Burner2k

Actually, Cables are capable of resisting Tension loads only. Personally, I've never modeled cable structures in FEA but I can think of a couple of ways in which it could be represented.

1. Use regular beam elements (CBAR or CBEAM) with DOF release option. Essentially, this option will tell FEA solver that you want the beam element to not resist specified DOFs. For example, you can release TY, TZ, RX, RY & RZ DOFs on each node of beam element. So the solver will *apply* only TX (axial) stiffness to your beam element which would simulate typical cables behaviour.

I am sure if you search on this forum or in general, you will find tutorials or videos on how to specify & define DOFs release.

2. Use CGAP elements. I believe you can specify stiffness values in PGAP for compression & tension. In your case, you will make the compression stiffness value 0 and enter tension stiffness value only. To calculate axial stiffness, use the formula EA/L...for unit length, the expression reduces to just EA i.e. value of Young's Modulus in to Area of Cross-Section of your cable. I would suggest you to read up on usage of CGAP/PGAP elements.

Quick internet search led me to these non-altair links. I am pretty sure there are good documentation from Altair as well on CGAP/PGAP elements.

https://knowledge.autodesk.com/support/nastran/learn-explore/caas/CloudHelp/cloudhelp/2019/ENU/NSTRN-Reference/files/GUID-13853503-EF40-4D01-A1E3-988C54BEEA64-htm.html

Okay on 2nd thought: Some one has posted cable query right on this site:

https://community.altair.com/community?id=c886883a1b2bd0908017dc61ec4bcb18

Hope the above helps.

Do simple tests using the above elements. Simple enough where you know the forces in your cables through hand calc and verify the same in your FE model. Once you get a reasonably good hang of the elements usage & confidence, the same can be applied to your actual model.

Burner2k

I tried both the methods on a couple of very simple problems and the results matched with each other as well as my hand calc values. I will try to post the input deck files some time this week.