Constraining the propeller in normal modes analysis

[Anonymous]

I was doing a tutorial from Nastran In-CAD Help:

http://help.autodesk.com/view/NINCAD/2017/ENU/?guid=GUID-955C0CC4-0F0E-42B4-8704-00A35A7AD14B

In 'Apply the Constraints' section we are fixing the lower center hole surface of the propeller, restraining it from moving and rotating in each directions.

My question is:

why we are not letting the propeller to rotate in one axis (in this case to rotate about lower center hole surface axis, probably it was X axis. I don't have access to Nastran In-CAD right now so I don't have how to check it in the model)? I was thinking that in normal modes analysis we need to constrain model, so we simulate its behaviour in real world. The propeller is rotating about its center axis and that's how I think it should looks like.

However, when I let the propeller to rotate about its center axis and run normal modes analysis the results are the same as in tutorial linked above.

Could someone help me in understanding this situation?

[Anonymous]

Hi Marcin,
it'related to the way normal modes are calculated. When you compute eigenvalues if the model is under-restrained Nastran will calculate zero frequency and associated rigid body motion.
If model is completely restrained It will calculate non-zero frequency and associated mode shape.

Indeed in your case you get a result even if you don't restrain rotation about x axis. If you check mode 1 you Will find a zero frequency (or in the order of 10-5) and mode shape will bè rotation about x axis. Mode shape 2 will be similar to mode shape 1 shown in the tutorial and possibly also associated frequency. There might be some difference since restraints affect calculated frequency and make model stiffer.

Alex

[Anonymous]

Thanks Alessando for your explanation.

I tried to achieve results you described in your post by doing again analysis with RX rotation allowed (there should be one ~0 Hz frequency in results) and another one with all rotations allowed. Results are these same like in case where whole shaft is fixed. You can see it in link below:

Higher resolution: http://img.pixady.com/2017/12/214379_0c35c1f1f368c.png

Sorry for stupid questions but I want to understand how it works... I thought that now I will get some 0 frequencies, but I didn't get it.

In real-world scenario if you will have to make a modal analysis of some rotational machine parts how you will constraint it? By fixing it entirely or by allowing them to rotate about its rotational axis?

[John_Holtz · Accepted solution]

Hi @Anonymous

The issue is this: solids do not rotate

Since they do not rotate, applying a rotational constraint has no affect on the analysis.

What happens with a solid is that the nodes translate in X, Y, and Z. It may look like it is rotating, but it is not rotating. In this image, I replaced the round hole with a square hole to make the motion easier to visualize. The arrows show how the corners of the hole are translating in Y and Z.

Solids do not rotate!

So, all of these constraints on the center of the hole are identical:

• Tx Ty Tz
• Tx Ty Tz Rx
• Tx Ty Tz Rx Ry
• Tx Ty Tz Rx Ry Rz

In the case of the propeller (and most "rotating" equipment), the propeller is fixed to the shaft. So relative to the shaft, the propeller does not rotate. Therefore, Tx Ty Tz is the correct constraint to apply to the hole.

If you had a situation where the model was really pinned so that it could spin freely, what you would do is create a rigid body connector inside the hole. This creates "spokes" from the center point to the nodes on the surface of the hole. You would then apply the constraint to the center point.

[Anonymous]

I am very thankful John for your explanation. I've read about degrees of freedom in certain elements but I had problems with understanding it. Now it is a lot easier.