linear sress analysis - multiple load cases in a row

[Anonymous]

Hi guys,

i have a common question. I created a curved beam with a gear on it in Inventor ´15 Pro.  I want let slide the gear above the curved beam and let the programm calculate the bend of the beam and the reaction forces.

I want to calculate it with an "linear static" analyse-method. My problem is: How can i tell the programm, that i want (for an excample 10) points of contact between the gear and the beam and calculate there my solution? In MES-Analysis method i can make it with time steps, but how can i make different load steps on different points of the beam in static linear? 

Here is my problem from the first place (actually in german) 

Thank you a lot! 

Greetings Tomatello

[AstroJohnPE]

Hi Tomatello,

In linear static stress, you would want to select the nodes ("Selection > Select > Vertices") at the first location and apply a force to those nodes. When defining the force, you can assign it to a load case. So for the first location, you would use load case 1. Then repeat it for each of the other locations and assign the force to the next load case. (Be sure to divide the total force by the number of selected nodes, which is shown in the title bar of the dialog, since each selected node will receive the force magnitude that you enter.)

That is all that you need to do for your example, but you might want to go to "Setup > Model Setup > Parameters" and "Add" a row to the load case multipliers table for each of your load cases just so that you can add a description for each load case.

[Anonymous]

Thank you so far AstroJohn.

What i missed to say is, that i dont have (or want) external forces in my system. 

I want to let slide the gear above the curved beam an let calculate the reaction forces by interaction of gear/beam.  

For that case, it would be great, to pull the gear to the point where i want to measure and repeat that (maybe with that multiplers table?).

Your suggested solution imlplied a force,that i dont know..

greetings tom

[AstroJohnPE]

Hi Tom,

Your desired solution method is not possible in linear stress. The assumption of linear stress is that the motion and displacements are so small that they have no affect on the displacement, direction and location of the forces, and so forth. So even though you could use a prescribe displacement to move the gear from the right end to the left end, analytically the forces would still be transmitted at the right end.

So your options in linear stress are to perform separate analyses with the gear in different locations, or a single analysis with nodal forces assigned to multiple load cases. As you mentioned previously, you can use MES and simulate the motion of the gear, but that will make the anlaysis much lengthier.

[Anonymous]

So that means, that i have to move the gear by hand in inventor and always have to convert it in mechanical simulatin step by step?

You said, that the linear stress method doesnt fit for my desired solution method..maybe the nonlinear stress method fits better?

Thank you very much so far.. 

[Anonymous]

Edit: Maybe a static nonlinear analyse method would be the best middleway..are your first suggested solutions valid to that method?

Thanks a lot!

[AstroJohnPE · Accepted solution]

Guten Tag Tomatello,

I'm not entirely clear how the load is developed in your case, so that may affect whether some of the following suggestions are appropriate or not. From looking at the images in your original post on the Inventor forum, it looks as if the load is "simple". That is, the beam doesn't have gear teeth, so you may not be simulating the detailed interaction between the gear and the beam and getting contact stresses, side loads, and so forth.

Also, the goal of the analysis can affect how you want to solve it. If you are just after an "engineering" solution, then simplifications are often acceptable. If you want something that can be presented to a customer, then a more sophisticated approach may be acceptable so that it is easier to understand.

So, here are some possible ideas:

1. One model: multiple gears. Assuming that you know what the load is and are willing to use nodal forces applied to different load cases, you could include multiple gears in the Inventor model for each of the locations. These "dummy" gears would only be used to show the location  as the gear "travels" along the beam; the nodal forces would be creating the load in the beam. By selectively hiding the different gears in the results, you could create images that appears to show the gear at different locations on the beam, and the effect on the beam. (You do know what the equivalent load is because you can run one analysis with all of the required details to get the load.) I have often added additional parts to my analyses to show other sections of the whole assembly even though these other parts do not interact with my real model.
2. Multiple models: one gear. Use separate models in linear static stress with the gear in a different location in each model. This requires a lot more work on your part (setting up multiple models), and trying to make images where everything is in the same location (same zoom, pan, view angle, etc) becomes tricky. (You can use a "presentation" from one model as the view for another model, so it may be possible.)
3. One model: one gear. As you mentioned, nonlinear static stress would let you move the one gear in the model to the different locations. This solution may be faster than an MES analysis; in theory, the gear can "jump" from one location to another in one time step. But you need to be somewhat careful in a nonlinear static model because it needs to be statically stable, and you cannot always depend on surface contact to provide the vertical stability. So, you might need to use "weak springs" to hold the gear vertically in case some iteration decides that the parts are not in contact.
4. One model: one gear. Nonlinear MES would be the "ultimate" solution. You could simulate the part rolling or sliding on the beam. It would make a great animation. The downside is the analysis runtime is longer because of the number of time steps necessary for the software to accurately calculate what happens as things move.

[Anonymous]

Guten Tag AstroJohnPE, 😉

i assume your suggestion as common solution 🙂 

First, my problem in short version:  I want to get a  reactionforce (appplied from beam/gear, which is a linear force in according of the displacement of the gear/beam) of the system (in horizontal way) which i can set up with the material data and the geometry of the beam. For that, solution 1 doesn´t fit for my problem.. well, solution 2 is a lot and inconvenient work. 

Solution 3 or 4 fits more for my claims. 

for that case, i have a few common question:

- To display the horizontal reactionforce, i selected some node-points and make a plot (against the time). What means the "integrate" action in the settings of the plot? The force against the displacement? 

- Is it correct, to assume, that it doesn´t make a difference of the reactionforces, if i fix the beam and let the gear roll over it or i fix the gear and let slide the beam above it?

 - What does you mean with "weak-springs" ?

- Is it possible to set boundary conditions, for an example, fix the beam on both ends in horizontal and vertikal way, and don´t let emerge frictions there? ( I want the frictions -> reactionforces at the point gear/beam) 

Thank you for your advices 🙂

Greetings 

-Tomatello

[Anonymous]

Hey Everyone,

I think you are about your assumption.. According to me simulation mechanical is used for local or within-network remote solving...

It has  some  chracterstics:

Simulation mechanical is fast , accurate and flexible for tools, Validate product behaviour before manufacturing..

Thanks,