Populating Beam Properties

[BEC_Kevin]

All -

I am working on a 2D "beam" structure using beam elements, composed of approx 50 members. Most of the beams are the same construction. When I highlight the similar beam members, right click, edit, element data, I get an error stating that I can only populate element properties for one element at a time. WHAT GIVES!?

Is there a trick or over-ride to this? All the beams are oriented properly (I, J, K nodes). When I manually enter all the data, it is all the same across the line for the matching beams. Further, I plan to optimize the structure, so I intend to change the beam properties several times.

I have made a library of the sizes I will use, so it is only a matter of a couple clicks per element... but 50 elements, several times.... I do not get paid by the hour! Any suggestions to help speed this up would be greatly appreciated!

Thanks in advance.

[AstroJohnPE]

Hi Kevin,

It sounds to me that you have each beam "element" in a different part number. If that is true, then that is a problem/disadvantage. The only reason that different parts are required is if the material properties are different. (There are other advantages, but they are not a requirement.) Different cross-sections can be entered by putting the beam elements on different layer numbers. (Just like you used different surface numbers to control the orientation, or at least I presume that is what you did.)

P.S. The warning message says that you can edit one part at a time; not one element at a time. If you have 50 members, I assume you have 200 to 1000 beam elements.

[ilyas_drawbridge]

Hi,

I don't know why it is not possible to edit multiple beam element parts simultaneously, but here's a workaround.

1. Set your Element Definition for one of your many similar cross section parts.

2. Right-Click on the part name in the tree>Copy>Element Data

3. Select (from the tree) all your other parts that you intend to input with the same element definition>Right-Click>Paste>Element Data

You should be able to accomplish your goal with just a few extra clicks. Alternatively, you can just change the line attributes such that every element with the same cross section are of the same part number. Select lines>Right-Click>Edit Attributes.

Regards

Ilyas

[BEC_Kevin]

Thank you for the replies! Worked like a charm! I perform a lot of plate/solid model analyses, this is the first time running beams. I am used to each "member" having its own part in the tree, so that is how I approached it.

Again, much appriciation! This saves a ton of time!

[FAB.Innovation]

The cross sectional Beam Properties required to deffine a beam are confusing for me.

When I create a cross section in Inventor, I can then go sketch mode: properties and Inventor calculates the cross sectional properties.

Unfortunately the way the sectional properties are shown is different to Sim Mechanical. 

I would like an easy mapping from Inventor to Sim Mechanical.

As best as I can see:

Area = a

J1 = Polar M of I

I2=Inertia Tensor Ixx

I3=Inertial Tensor Ixy

S2=?

S3=?

Sa2=?

Sa3=?

I also have an assymetric section however this is restrainted so that it cannot rotate. Section 3 of attached.

Can you please look at the section and advice the data to be inputed into Sim Mechanical.

Thanks

[AstroJohnPE]

Hi FAB,

Just in case you did not discover this, when you have one of the cells for the cross-sectional properties selected on the Element Definition spreadsheet, the "Cross-Section Library" button is active. When you click on the button, a new dialog appears. The software will calculate the cross-sectional properties for the square tube, "channel", and I-beam based on entered dimensions. So that only leaves the odd-ball sections.

• A in Mechanical = Area in Inventor
• J1 in Mechanical = nothing in Inventor. You will need to do this calculation manually. The book "Roarks Formulas for Stress & Strain" may be the best reference.
• I2 in Mechanical = Ixx or Iyy in Inventor, depending on how you orient axis 2 in Mechanical versus the orientation of the section in Inventor.
• I3 in Mechanical = Iyy or Ixx in Inventor, depending on how you orient axis 2 in Mechanical. Note that you may have made a typo in your original message when you wrote I3 = Ixy.
• S2 in Mechanical = nothing in Inventor. You will need to do this simple calculation manually. S2 = I2/(distance from the centroid to the farthest location in direction 3).
• S3 in Mechanical = nothing in Inventor. You will need to do this simple calculation manually. S3 = I3/(distance from the centroid to the farthest location in direction 2).
• Sa2 and Sa3 = nothing in Inventor. These values are normally not required unless your beam member is very short compared to the height and width of the cross section. If that is the case, you need to calculate Sa2 and Sa3 manually, or use a solid model if possible for those members.

I suggest you read the page titled "Beam Elements" in the online Help. There are two such pages: one is for linear analysis, and the other is for nonlinear analysis. I assume that you are doing some type of linear analysis.

FYI: I am working on a spreadsheet that would let the user enter each length and width of the edges making a cross-section and calculate the above parameters (except for Sa2 and Sa3). The torsion resistance J1 is tricky for a general cross-section, so that is where I am stuck currently. It may be quite a long time before I finish it, but feel free to send me a private email through this discussion forum sometime in the future to ask if I am done yet.

[FAB.Innovation]

Thanks you John.

Now that Autodesk own Algor it really seams like a good idea that the sectional properties in Inventor can be transfered over to Simulation Mechanical..Perhaps a SP2 request.

Thanks you again.

FAB