topic Re: Rotational Force loading only for one part in Inventor Nastran Forum

Rotational Force loading only for one part

ghadyani — Mon, 25 Nov 2019 13:53:35 GMT

I am trying to simulate one rotation of a crank so that the arm and piston follow it.

I have set up a NLT analysis with some basic constraints. I have also added PIN constraints between piston and arm as well as arm and crank (yellow in the screenshot).

Piston is constrained to only move along its cylindrical axis
Arm (red) and Crank (yellow) have only one constraint to keep them from moving sideways.

I can't seem to be able to correctly apply loading or transient table to simulate one full rotation of crank and see what happens to rest of part.

How does one go about setting this up?

Any hint is appreciated.

I have attached the model files to this post.

Re: Rotational Force loading only for one part

John_Holtz — Mon, 25 Nov 2019 19:46:09 GMT

Hi @ghadyani

A nonlinear transient response analysis in Nastran either cannot perform this analysis, or it is very difficult to get it to do what you want. The main reason is this (assuming you are duplicating the setup from Simulation Mechanical): you want an enforced motion to indicate that the crank rotates X degrees in T seconds. A nonlinear transient analysis does not support enforced motion loads.

A "Rotational Force" is a centrifugal load. It tries to stretch the model in the radial direction based on the speed (RPM or equivalent units) and rotation axis. This is not the type of load that you want for this analysis.

The other problems with your setup is that Pin constraints that you applied to the "joints" between the linkages are constraints that connect the model to the ground. You need to create a connection between parts that allows rotation. As far as I know, the only way to do that in Inventor Nastran (Nastran In-CAD) is the method described in this post: Pin and universal joint between bodies . The other thing that is required for a large displacement analysis is to change the rigid connectors to bar elements, as described in this post: Pinned connection in Autodesk Nastran .

If such an analysis can be performed in Nastran, it would require using the explicit solver (which was released as a preview in version 2020.1). I do not know if the explicit solver has all of the capabilities that would be necessary:

enforced rotation
rigid connectors (to create a portion of the pin connection between links)
spring connectors (to create the remaining portion of the pin connection between links)

Perhaps another reader knows that answer offhand. Otherwise, a test model would be required to test out the concepts (such as your piston model 😊).

Re: Rotational Force loading only for one part

John_Holtz — Mon, 25 Nov 2019 20:58:34 GMT

Hi @ghadyani

I am pleased to report that the explicit dynamics analysis can handle the piston analysis, with one minor difference than what I was describing before. Here is what you can do:

Rigid connectors do work in explicit dynamics and do use large displacement. The Parameter RIGIDELEMTYPE does not need to be changed.
Enforced motion (and in your case, enforced rotation) does work. Note that for the explicit solver, the enforced motion must not have a constraint in the same direction. This is different than the other Nastran analyses that require a constraint in the same direction as the enforced motion.
Spring connectors do not work for the "pin" between the connection. Beam elements do work for the pin between the connections.
1. Therefore, you need to create sketches in the modeling environment and draw lines that represents the pin between each of the joints. (If clever, only one sketch with two lines is needed in your model. One line for the crank-to-arm pin, and a second line for the arm-to-piston pin.)
2. Define an Idealization, set the type to bar or beam, and define the beam cross-sectional properties.
3. Create separate rigid connectors in each of the holes. Use the face of the hole for the "Dependent Entities" and the end of the beam/sketch for the "Select Point".
4. Define an End Release on the beam to allow the joint to rotate. That is, the pin is in a bushing or bearing, to the beam/pin must be free to rotate relative to one of the links. (Of course, "weld" the beam to one of the links so that the beam is not free to spin.)

In my model, I worked my way up from rotating just the crank to rotating the crank and arm. See the attached model "explicit dynamics (version 2020.2).zip" and animation "piston animation.zip". I was using version 2020.2 of Inventor Nastran.

Re: Rotational Force loading only for one part

ghadyani — Tue, 26 Nov 2019 12:31:39 GMT

Hi John,

Thanks for your reply and all useful links.

I won't be able to open your model since I am on 2019, but I will try your suggestions and report back.

EDIT: As you said your solution is only applicable to 2020.1

Re: Rotational Force loading only for one part

ghadyani — Fri, 29 Nov 2019 13:32:30 GMT

Hi John,

Thanks to your post and links, I have learned a lot when it comes to this kind of simulation.

I just wanted to verify that everything I am doing is done correctly before moving to a full assembly. So I just analyzed the crank part only under a 45-degree rotation. However, I ran into two issues:

when I look at the results the crank is definitely not rotating 45 degrees. I guess I have to tweak some time-load tables but I am not sure exactly how to do it to get a 45-degree rotation go from workpoint to actual part.
There seems to be some stresses around the "solid connectors". Is this because we are simulation our pin support using rigid connections

Re: Rotational Force loading only for one part

John_Holtz — Mon, 02 Dec 2019 15:36:18 GMT

Hi @ghadyani . You are making progress 🙂.

Your guess is correct. The Transient Table Data (Table 1) for the enforced motion indicates to rotate the part 45 degrees in 1 second. 45 deg/sec * 0.01 duration = 0.45 degree total rotation. The results look about correct for that.
There is a force (or torque) to accelerate a part for a stand still to a velocity of 45 deg/sec, and then there is a reaction force to the centripetal motion. The forces result in a stress.

Note: the constraint that is named "Necessary?" is not necessary. The rigid connectors prevent the nodes on the inside of the hole from moving the Z direction.

Re: Rotational Force loading only for one part

ghadyani — Tue, 03 Dec 2019 01:33:55 GMT

@John_HoltzThanks for explanations, this clarifies the issues.

In spirit of replicating tutorials for Simulation Mechanical, I'm going to post another question on how to have actuators (hydraulic/pneumatic) in Nastran.

Re: Rotational Force loading only for one part

eggheadkhan — Mon, 20 Jul 2020 08:00:25 GMT

@John_Holtz

Can you please check this still works in 2021.0.0.401?

I get a message saying cross section not available (for beam idealization) for explicit...

(as per your recommondations & the pin guide)

And when I run the examples I don't get the animation outcome...

Re: Rotational Force loading only for one part

John_Holtz — Mon, 20 Jul 2020 15:45:18 GMT

Hi @eggheadkhan

The explicit analysis type is different in many ways, so some instructions in the articles do not apply directly.

There are three options for defining the beam cross-section properties. You have tried 1 and learned that that does not work for the explicit analysis. You only have two more options to try! (Hint: use the "Property Input".)

Re: Rotational Force loading only for one part

eggheadkhan — Mon, 20 Jul 2020 23:26:13 GMT

hi @John_Holtz , thanks for your reply.

to be honest, I played a lot of whack-a-mole over the weekend, and for the project on my desk, I hired someone to do it for me.

I learnt that the explicit solver only likes to use 1x Xeon 8168 when 2 are available, and doesn't like AMD 7742 (at least on win10), plus a few other things 🙂

but what I'd like to learn is how to replicate that animation of yours somehow... is your attachment above ready to go for inventor nastran 2021.0.0.401? (the crank and the arm moved a little, but even increasing the duration 10x, seemed to just bend the crank beyond that point)

Re: Rotational Force loading only for one part

John_Holtz — Thu, 23 Jul 2020 17:04:02 GMT

Hi @eggheadkhan

Regarding AMD processors, please see this forum post: https://forums.autodesk.com/t5/inventor-nastran-forum/inventor-nastran-explicit-solver-will-not-work/m-p/9511257

The 2020.2 model that I provided runs the same in 2021.0. You may need to do these items:

Set the deform option scale to Actual instead of Percent.
Use the proper command to create the animation. See "Animation does not match the individual results of an In-CAD analysis".

If extending the duration, be sure to extend the "Transient Table Data" for the enforced motion load. Otherwise, the crank will get to 0.1 seconds and stop (which is the end of my load curve). The explicit analysis does not appear to extrapolate the load curve table. I ran the analysis for 2 full revolutions of the crank arm. A nice little out-of-plane vibration starts to occur on the second revolution, so it will be interesting to see what happens after 10 full revolutions.

Re: Rotational Force loading only for one part

eggheadkhan — Fri, 24 Jul 2020 09:09:30 GMT

@John_Holtz

it didn't quite make all 10, the first one is useful, then we go to a "explicit" 🙂 dance...

thanks for the reply.