Simulation Mechanical 2014- Analysis 2D

[michalbaran3]

Hi.

I have a question. How can make revolution in Analysis 2D? I want make revolution spur gear. In Attachments I sent screen of analysis.

[AstroJohnPE]

Hi michalbaron3,

You probably want to use a prescribe displacement to rotate one of the gears and define surface to surface contact between the teeth. Optionally, you can apply a resisting moment to the driven gear to simulate the load.

• For the prescribe displacement, see "Start & Learn > Learn > Tutorials", then "Analyzing and Evaluating Results Tutorials > Piston Mechanical Event Simulation".
• For the surface to surface contact, see "Start & Learn > Learn > Help", then "User's Guide > Examples > Mechanical Event Simulation > Surface to Surface Contacts". (I see that you have contact defined already, so you may not need this step, but others who read this thread may benefit from it.)

I'm not sure what constraint you have applied, so you may need to change it following the example in the Piston tutorial. The piston tutorial used the "Joint" command to create the spoke of beams where the shaft is. That command only works with 3D CAD models, but you can use the "Draw > Design > Contact Elements" command to generate the same type of lines in a 2D model.

P.S. Those are some really large gears! They must be heavy since it is a solid face. You should either accelerate them slowly, or define an initial angular velocity for each of the parts. If you were to start at time 0 with no initial velocity and instantaneously rotate them at N rpm, the inertia will lead to huge stresses and problems with the surface contact, etc.

[michalbaran3]

Thank you for your help. I tried to do as you wrote "Draw> Design> Contact Elements". The first gear started rotate but the second gear no. I sent attachment with simulation in Simulation Mechanical. If you can help me and show how do it. 

[AstroJohnPE]

Hi,

Unfortunately, the .FEM file that you provided in only a portion of the input. What you need to do is create an archive ("File > Archive > Create"), change the extension from .ACH to .ZIP or .RAR, and attach that to your reply. There is a thread somewhere in the discusion forum that goes into details about creating and posting archives. (I have a newer version of Simulation than you are using, so even if I did complete the input, you probably would not be able to open it.)

But in general, if the driven gear passed through the other gear without causing any stress or evidence of contact in either gear, there is a problem with the surface contact.

[michalbaran3]

Sorry, I didn't know. Now I sent with extension .ACH

[AstroJohnPE]

I think your problem is still with the scale (size) of the model. You are trying to rotate a 209 inch pitch diameter gear with an 82 inch pitch diameter pinion that is driven by a beam only 0.16" in diameter where the 15 inch diameter shaft is located! There is so much inertia in the pinion (approximate weight = 1500 lb = 6700 N) that the beam (really a "wire") is twisting up without moving the pinion, let alone rotating the mating gear. Check the "Results Contours > Displacements > Rotations > Magnitude", and you can see that the end of the beam at the prescribe displacement is rotating (57 degrees when I stopped the analysis), but the end connected to the pinion barely moves (3E-6 inch).

I made these changes and got the system to behave as expected:

1. changed the filename. (Probably not necessary, but non-english characters in the filename concern me)
2. added more beam element "spokes" so that each node around the circumference of the gear and pinion was connected to the center point.
3. coarser mesh (so that the analysis would run faster while troubleshooting)
4. changed the model units to mm so that the gear and pinion would be 209 and 82 mm diameter. Note that when you change the model units AFTER you have entered input, ALL of the input should be checked and updated, such as the material properties, gravity constant, beam cross-section properties, etc.
5. set gravity constant to 0
6. made the beam elements 20 mm diameter and set the mass density to 0 so that the inertia of the "stiff" beams would not affect the results.

[michalbaran3]

Thank you for your help. Now the system is working properly but there's one problem. The gear has no stress on the teeth. Why? The pinion is ok.

[AstroJohnPE]

Just to be clear, the gear has stress but they are very low (larger than 0.0007 N/mm^2 but probably less than 16 N/mm^2). If you isolate the gear (right-click the part in the browser and choose "Isolate"), you will see the stress distribution in the gear using the full range of color.

Assuming that the gear does indeed have stress, reasons that they are so low might be one of the following:

• The gear is much thicker than the pinion, so the same contact force between the teeth divided by the thickness results in a lower stress. Check the type of geometry (plane stress or plane strain) and thickness in the Element Definition.
• Check the material properties.
• You can also check the reaction force. I'm not sure what this will tell you about the analysis, but perhaps it will help point to the problem. Depending on how closely the nodes align between the contacting teeth, the force at a node can be higher on one side than the maximum force on the other side; that is, the total force is equal and opposite, but when distributed among different nodes, the maximum may be different. You should see the reaction force changing with each time step.

Let us know what you find!

[michalbaran3]

In fact, if I isolate the pinion I see the stress distribution in the gear approximately 54 N/mm^2 while the stress distribution in the pinion is approximately 900N/mm^2. The gear is the same as thick as the pinion. The material pinion and gear is the same( Steel ASTM- A242). I havn't idea how to do to stress were the same. I sent my analysis. 

[AstroJohnPE]

Actually, the gear and pinion are different thicknesses which explains why the stresses are different.

• The pinion is set to a geometry type of "plane stress" and has a thickness of 0.039 inch (1 mm).
• The gear is set to a geometry type of "plane strain", and therefore the thickness is 1 inch (because the unit of length is inch in the model units). The processor uses a thickness of 1 for all plane strain parts. The user-entered thickness of 0.039 inch (1 mm) is ONLY for visualization purposes in the Results environment, as indicated on the dialog. The user-entered thickness does not affect the results of a plane strain part.

I suspect that you would still see a difference in the results even if both thicknesses were 1 inch because of the difference between plane strain and plane stress.

• plane strain = strain (displacement) occurs in the YZ plane only. The X strain is 0. Due to Poisson's effect, there are stresses in the X direction which you can see by using the "Results Contours > Stress > Tensor > XX Component"
• plane stress = stress occurs in the YZ plane only; the stresses in the X direction are 0. Due to Poisson's effect, there are displacments in the X direction, which strangely the software does not show.

[michalbaran3]

Thank you for your help. Now everything is working properly!

PS. 

I have another question. How to thicken the mesh only from the edges of the teeth?