Can't manage to make a gear analysis to work from a Solidworks assembly

  • 133 Views
  • Last Post 20 February 2019
  • Topic Is Solved
3enrique posted this 09 February 2019

Hello,

I have modelled a simple gear train in Solidworks. It does work there as I can use its basic modion analysis. However, when I've tried importing the model into Ansys and analyse it there it gives several errors and doesn't work. All I want is to rotate the first gear at 35 RPM and look at the stresses experienced in the connections but after days of trying I don't know how to do it.

Here are the files, if someone is able to help me.

https://drive.google.com/open?id=1-RwX8wxT2mFLl9YWbjVWpSvZFc8LKEGl

The assembly I'm trying to analyse is "Ensamblaje13 - simple.SLDASM"

 

Thank you very much for any help!

Order By: Standard | Newest | Votes
peteroznewman posted this 09 February 2019

 Hello Enrique,

The geometry and speed of the first gear is not enough information to analyze the stress  in the parts.  You also have to specify the torque or moment that this gear train is working against, otherwise, it is an unloaded gear train that does no work.

Please reply with information about the load the gear train is working against.

Regards, Peter

3enrique posted this 09 February 2019

Thank you for answering, it's my first time working with gears so I'm a bit rusty. The first gear (highlighted in blue) should be rotating at 35RPM and experiencing a torque of 3.157 Nm

peteroznewman posted this 09 February 2019

You mentioned the input torque at one end, what is the output torque at the other end?  Why do you need the idler gears? Did that come from a space constraint?

The shapes you show above don't look like practical gear teeth, there is no space between the tip of the tooth on one gear and the root of the gear hub on the mating gear. There should be a fillet radius at the base of the tooth to avoid a stress concentration. They also don't look like the teeth have an involute profile. Gear design is a special design task. What do you need to analyze?  It's pointless to analyze the stress in this geometry, these are not real gear teeth.

  • Liked by
  • Jackely
3enrique posted this 09 February 2019

It is not my gear design but the task is to analyze it and give feedback resulting from it. The fillets will be added later in order to compare both results. The last gear is connected to a shaft which will just rotate a shaft with a disk on top to measure the output speed.

peteroznewman posted this 09 February 2019

I think the analysis you are being asked to do is to calculate the output speed given the input speed.  That is a simple calculation on a spreadsheet using the pitch circles of the gears.  You can ignore the teeth, since they are not authentic gear teeth, just a visual outline to show that there are teeth. Do you need help calculating the output speed and direction?

I downloaded your SW files, but I'm on SW 2017 and you have a newer version, so I can't open it. Neither can SpaceClaim 19.2. You need to Save As an older version of Parasolid and provide that file. You can attach a zip file containing the Parasolid file to your reply.

I provided a lot of feedback on the tooth design in my last paragraph of the previous post.

3enrique posted this 10 February 2019

I already did the calculations for output speed but now I need to know the stresses in each gear and where the max occur. I tried to save the files in an older format but the links of the assembly just break. I have however also included a save of the assembly in IGS format in the Google Drive which seemed to solve some, but not all, of my problems in Ansys. You should be able to open and operate in Ansys.

peteroznewman posted this 11 February 2019

You don't need the gears to spin to calculate the stress in the teeth. Just fix the last gear and apply the input torque you were given to the first gear. You will need to create revolute joints on each gear center and contact between the teeth on each gear.

It would be much less work if you do a hand calculation to determine which gear mesh has the highest force going through it, and just analyze that one gear mesh for stress. You will then hold one gear fixed and apply the calculated torque to the other gear.

3enrique posted this 11 February 2019

Which type of contacts should I use for the teeth? And for the supports? I have been trying to use No separation Behaviour and Frictionless Supports but it seems its not working as in the results the first 3 gears appear to be moved vertically and the rest are fixed without having experienced any stress.

peteroznewman posted this 11 February 2019

Use frictional or frictionless contact on the teeth.  Use a Revolute Joint on each gear shaft hole. Don't use No Separation contact anywhere.

3enrique posted this 12 February 2019

I'm still stucked. I added frictionless contacts on the teeth and a bonded contact for the two gears which are stucked together. I wasn't able to add a joint in the shaft holes as there isn't any "base surface" like a shaft, just a mobile location (the shaft hole). First I added frictionless supports at the holes but some gears just moved upwards. I then added fixed supports but it doesn't seem to have worked as it just shows some minimal stress in the middle gear and no movement.

Sorry for all my questions, it is quite important for me and I'm feeling a bit overwhelmed.

peteroznewman posted this 12 February 2019

Don't use Fixed support anywhere but on the ID of the last gear.

Every other gear has a hole (or a shaft) through the center. That face is what you pick to make a Joint to ground, type = Revolute.

You are correct to use Bonded Contact between the gears stacked on the same center. Another approach is to unite the solids in the CAD system so they become one body.

3enrique posted this 13 February 2019

It is giving me a not enough constrains error. I have frictionless contacts between gears and cylindrical joints to ground (didn't see any revolute type) at all shaft holes except the last one which has a fixed support.

I tried to add frictionless supports on the upper and lower surfaces of the gears to see if this solved the problem but although it removes the error the gears will just not spin.

peteroznewman posted this 14 February 2019

You will not see the gears spin in this model. When you make the last gear fixed, that means nothing is going to turn. You apply a Moment load to the first revolute joint and the contact force through the teeth carry the torque to the next gear and the next gear and so on.

RMB on the Connections Folder and Insert Joint, then set the joint to Body-Ground, then set the type to Revolute, then pick the cylindrical face.

Did you do the hand calculation of the force on the gear teeth of each mesh?

3enrique posted this 14 February 2019

This is what I'm getting for the first gears:

It seems very small but it may be correct as the moment is just 3Nm. How would I go on to make the hand calculation you comment?

 

I don't know if it will help, but this is my Anys file:

https://drive.google.com/open?id=1eU59d0RhbFlrmEGLH9c3pfnpi-ydL-4I

 

Thank you very much for everything once more.

peteroznewman posted this 14 February 2019

Ah, now I see why you couldn't find a Revolute Joint, you're using AIM 19.2  not   ANSYS Workbench 19.2.

AIM has a simplified User Interface so Joints are not exposed. Each gear needs two Frictionless Supports, one on the Cylindrical Face and one on the Flat face to make the equivalent of a Revolute Joint. I believe you can open Workbench and Mechanical to exposure more functionality, but then you are in a totally different User Interface.

To do a Hand Calculation (which gives you an estimate, not an exact value)

  • Draw a series of circles with a radius of half the tooth height and are tangent to one another.
  • This method uses the simplifying assumption that the force is tangent to the pitch circles you just drew (it isn't).
  • This method uses the equilibrium argument that the force at the tooth interface has to be equal and opposite.
  • The force on the first tooth from the input torque is F.in = T.in/R.in
  • Take that force and use it through the gear train. The force will be the same on the two idler gears.
  • The force changes on the stacked gear. It is the same F.in on the tooth of the small gear, but it is smaller on the tooth of the bonded large gear. This uses static equilibrium.
  • F.out = F.in*R.small/R.large
  • That tooth force, F.out is on each tooth to the last gear.

What this tells you is the stress on the teeth go down after the stacked gear. You could "Remove for Physics" in the Geometry editor, all the gears except the first and second gears and just look at the stress on those two teeth by putting the fixed support on the ID of the second gear.

I tried to use AIM 19.2 to do my own two gears, but had issues with it finishing its tasks.  It solved completely, but even leaving it overnight, it can't finish post-processing the results. The transcript  also shows it solved.

I removed teeth from the gears to allow more elements to be used on the teeth in contact.

Obtaining the stress is just an exercise in button pushing because these are not real gear teeth, they are not even close.

  • Liked by
  • Jackely
3enrique posted this 14 February 2019

I have tried to do it on workbench now and although I have found and inserted the revolute joints, I am getting errors. I have also inserted frictionless contacts between gears and bounded contact between both stacked gears.

Here is the file: https://drive.google.com/open?id=1U1HYj3MgKq8keSl241HTxouZUAW8qE40

peteroznewman posted this 14 February 2019

Attached is my ANSYS Workbench 19.2 example of two gears, with a torque on one and fixed on the other.

 

Attached Files

3enrique posted this 14 February 2019

It seems I'm not able to open it due to it having be saved in a newer format. I'm using Ansys 19.1

peteroznewman posted this 14 February 2019

That is correct, you can't open newer release files in older release software.

I tried to download from your link but found you only put the .wbpj file and you didn't make an archive that is the .wbpz file.  The .wbpj file is useless on its own. Please create an archive file.

3enrique posted this 14 February 2019

Sorry, should have known. Here it is: https://drive.google.com/open?id=1seWwHh1kgvTcnqImtLOuz2HQiniRsdUq

peteroznewman posted this 15 February 2019

In the CAD, all the gear teeth have to be oriented so they are touching in the direction that the load is going to transfer the force. In your first mesh, there is a 0.5 mm gap.  You have to rotate one gear to close that gap before ANSYS can solve the stress in a Static Sturctural analysis.

Look at this other thread that has gear teeth in contact.

3enrique posted this 15 February 2019

Thank you that seemed to solve the error, though I'm still getting some warnings. I am also not sure that the result I'm getting is correct, though getting one is a big step.

Here is the file: https://drive.google.com/open?id=1uj66xEZvo_4nTGjCZD6H7smMxnsq5IU5

peteroznewman posted this 15 February 2019

Here is a simpler version of your model with just two gears. Look at the first Revolute. The Z axis, which is what the rotation is about, is pointing in the wrong direction! It has to be aligned with the cylindrical face axis. It is not at the center of the gear. You have to pick two faces to get it to snap to the center.

In the image below, the Reference Coordinate System under the Revolute Joint has a new center and new direction for the Principal axis.

I put a fixed support on the ID of the bottom gear since I suppressed the last gear that had a fixed joint. 

You won't get good stress results with such a coarse mesh compared with a fine mesh.

If you have the Student license, you have to keep the nodes < 32,000 to be able to solve.

Just work on two gears initially.

You can use a Joint Load of type Moment instead of a Moment. Either one will work.

Insert an Contact Tool under the Connections folder. Generate Initial Contacts. Use Adjust to Touch on the contacts that are Open.

Under Analysis Settings, Turn on Auto Time Stepping and set Initial Substeps to 10.

Turn on Large Deflection.

If you have 3 gears, then you will get a better distribution of stress on the second gear.  You could simulate the third gear by putting a remote displacement on one tooth face on the opposite side, and use the revolute joint on the second gear (not fixed support). This is more realistic for the idler gear.

All of this is in service to learning the process, because these are not real gear teeth, there are sharp interior corners so the exact value of stress is infinity.  Do some research on Stress Singularity using the site Search capability.

  • Liked by
  • Jackely
3enrique posted this 18 February 2019

Thank you very much once more. I've followed all your steps and managed to reach a solution which makes more or less sense for the model with 3 gears. However, I'm getting a different result to yours. Could you check if I've done something wrong?

 

https://drive.google.com/open?id=1WXVobNPLd0LlogumBWPvUgVeJoSZB4xZ

peteroznewman posted this 18 February 2019

Please reply with an image inserted showing stress on the same scale as I show above.

3enrique posted this 18 February 2019

This is what I'm getting. The file is in my previous post. Values seem too low to me.

peteroznewman posted this 18 February 2019

Make your legend exactly match my legend.

  • Change units from m to mm which will change Stress from Pa to MPa
  • The number between orange and red, type 0.3
  • The number between dark blue and light blue, type 0.025
  • Click on any color in between, see the + and - sign popup?  Click the + sign until you have the same number of squares as my legend.

Don't pay attention to the biggest number in my legend of 2.8 MPa and the biggest number in your legend, 1.2 MPa because I told you that this geometry has a stress singularity. That means the exact value of maximum stress is infinity. The smaller you make the elements the larger will be the calculated result. My elements are smaller than your elements so I get a bigger maximum value.

But when you make the color scale the same, look at the distribution of color. It should start to look similar.

3enrique posted this 18 February 2019

 

This is it. It does look very similar indeed, though there are some variations. Still not sure if mine is right.

peteroznewman posted this 19 February 2019

I downloaded your model. The mistake in your model is your contact type is set to Bonded. Change it to Frictional. Then the contours will look more like mine. You might experience some difficulty getting the solver to converge because Frictional contact is nonlinear, while Bonded Contact is linear. You might need to turn on Auto TIme Stepping and set the Initial Substeps to 10 or higher. You must also insert a Contact Tool under the Connections folder and check that the Frictional contact is closed. If it is not, you must use Adjust to Touch in the contact definition.

3enrique posted this 19 February 2019

This is what I have got now:

I think it's very similar, let me know what you think. I can't believe I had bonded contacts, I have done the same steps so many different times it must have slipped through. I made them Frictional contacts, though with 0 Friction Coefficient, which one did you use?

Show More Posts
Close