Gear generation from a rack

[stephenmcd74]

Hello everyone

I want to create specialised gear profiles, which cannot be done with Inventor's spur gear generator.

I want to draw/model the generating rack, and then use this in Inventor to generate a tooth. So effectively, this would be virtual hobbing.

It is possible with another well-known software - please watch the first 2 minutes of this video (sorry it's in French):

https://www.youtube.com/watch?v=ElKMmcrr3AY

Am I right in thinking that this is not possible with Inventor?

Many thanks for any help

Stephen

[TheCADWhisperer]

I don't

parle français

, so perhaps I am mistaken - but I did not see a demonstration of SolidWorks functionality - what I saw looked like a 3rd part app.

What I saw in the video can be done natively using the Dynamic Simulation>Trace functionality.  (no 3rd party software required)

[stephenmcd74]

Hello there Cad Whisperer

Thanks for your interesting reply.

Could you possible explain a little more about how this would work, as I’m afraid I have never used Dynamic Simulation/trace?

Are there any videos/tutorials anywhere of this kind of process, or of anything similar?

Thanks again

Stephen

[TheCADWhisperer]

Here is a short form video - not exactly the same, but the principle is the same.

The Trace is the easy part - proper setup of the Dynamic Simulation assumes expert level knowledge.

If you can attach your assembly here and it proves useful for something that I could use in my classroom, I could make a video using your geometry.

[stephenmcd74]

Hello again CW

That is a cool video, and i can see what you are getting at.

Yes, I could draw up the rack, and provide you with the details for your video - sounds brilliant.

However, one question sprang immediately to my mind while I was watching your rotary engine video: In that case, you use the trace of a single point to create the geometry that you then chop out from the engine block. However, to generate the gap between 2 teeth on a wheel using the tooth of a rack, it would be necessary to use multiple points on the generating tooth. Would this be possible? If so, this would create a complex mesh of lines - how would this be used to cut out the correct profile? Would I have to laboriously constrain a spline all the way around the web of lines?

Thanks

Stephen

[TheCADWhisperer]

I am going to have Inventor automatically create as many points (in a spline) as you tell me you want.  100? 1000? 10000?

The key for me is knowing your intended pitch diameter.

The video was just one specific application of Trace.

What if the point being traced was the continuously variable intersection of the rotation of pitch diameter circle and your "rack"? 

[stephenmcd74]

Ok CW

I am going to try to get this organised for you tomorrow, and send you the stuff.

Could I just ask you to give me as much detail as possible about exactly what you want sent, what format that should be in, and any other required data.

This really is great stuff - thanks so much for your help!!

Stephen

[stephenmcd74]

Dear Cad Whisperer

Please find attached a generating rack, as discussed. This is to produce a pinion of 16 teeth, module =1, and with an outside diameter of M(Z+2)= 18mm.

Is this enough to allow you to create the video? This is such a great subject that I'm sure it would be of much interest to your students, as well as to many other people.

Please let me know if you think the video will be possible.

Many thanks again

Stephen

[TheCADWhisperer]

I have a bunch of other work I need to get done first - so it might take me a while and  no guarantees, but I think you have provided all of the information I need.

I suspect Walter might come along and make some progress on this before I can get back to it.

ping @WHolzwarth

[WHolzwarth]

  Jeffrey, you're a dangerous guy ..

[stephenmcd74]

Hi there Walter

I fully appreciate that both yourself and the CAD Whisperer are very busy with all kinds of stuff.

However, I just wanted to say that if there is any possibility that either of you would have a little time to help me with this in some way, I would be ever so grateful.

I understand the principle which is demonstrated in the video from the CW, but it is not at all clear to me how this principle of using a single point to create the geometry to cut out can be extrapolated to use the motion of the rack tooth to cut out a corresponding profile from a wheel.

With sincerest thanks

Stephen

[TheCADWhisperer]

Edit: Put a surface body cylinder at the Pitch Diameter in the Gear.

Put an extruded surface body plane at the theoretical contact on the Rack.

Oh, and @WHolzwarth if you didn't catch this, iProperties indicates the OP is using Inventor 2015.  

Put the "Rack" into an assembly with one translational degree of freedom (this should convert to Prismatic Joint in Dynamic Simulation).

Put "Gear" blank cylinder in assembly (actually you might do that first) and place at appropriate distance from Rack.  Constrain with one rotational degree of freedom (this should convert to Revolution Joint in Dynamic Simulation).

Go to Dynamic Simulation and place Revolving Cylinder on Plane Joint.  (select the option without adding tangency as you already have it located)

Add appropriate driven motion to Rack or Gear.

Got that working?  Good!  If you can get this far - attach your assembly here.

Now figure out the Trace relative to the translational/rotation motion (I haven't thought that far ahead - this might be a bit challenging.)

[WHolzwarth]

I'm still busy with it, but you can see the way of doing.

[TheCADWhisperer]

I hope there is an easier way... ...that was not what I was thinking, but again, I have't put much thought into this yet.

I was thinking one point (might require a dummy part) with point sliding along rack edge while maintaining intersection with pitch diameter on the pinion.

Maybe Sliding Point on Curve .... you are drawing me into this problem and distracting me from the work that pays my salary...  .. I sure hope I can get a lecture/lab out of this...

[WHolzwarth]

In the end, I used another way. But the result seems ok.

2015 files attached

[stephenmcd74]

Dear Wh

That is absolutely brilliant!!!!!!!!

But please, please could I ask you for some details as to how exactly you have done this, as I'm afraid it is not at all clear to me?

If you could possibly just explain the individual stages which you have used?

As much explanation as you can possibly give me would be most gratefully received.

Really thanks a million

Stephen

[TheCADWhisperer]

---

@stephenmcd74 wrote:

Really thanks a million

Stephen

---

@WHolzwarth  I'll be expecting my 10% referral fee on that million.

Isn't it past your bedtime?  Kept you up working on this, didn't I.

OK, I'll take off 3% for your overtime.

[WHolzwarth · Accepted solution]

---

stephenmcd74 schrieb:

Really thanks a million

---

If we're talking about dollars, Stephen: It's too much. I won't be accepted for a free license of Fusion 360 anymore ..

What did I do? I've used two ways:

- Creation of traces (Points on rack vs. gear part), using DS. Problem is here, even if you create traces of many points, a hull curve must be done out of many points and curves. Lots of painful work.

- Second method was moving the rack as solid body through the gear, combining several positions into a subtract body, and doing a boolean cut vs the gear. This was done for a one tooth step, this region was cut out by splitting, and afterwars patterned to a complete gear again.

In this sample we have:

- Module 1

- 16 teeth 

- Pitch dia from that: 16 mm

16 teeth mean 22.5° angle from tooth to tooth. I split it into 10 steps. From tooth to tooth, the rack is moving Pi*1mm=3.142 mm.

Now the creation:

- Place rack as separate body in the gear (Copy object is the way to go)

- Angular pattern of the rack body 11 times (= 2.25° step) as separate bodies

- Move each of these bodies along it's length with a different distance (n*Pi , n=0.1,0.2, ..)

- Mirror these bodies. (Was too much work, combining them into a single body and mirror this would have been easier)

- Combine all to a single body

- After that only 2 bodies are left. A boolean cut is needed between gear and cut body. Result is gap for a single tooth

- Now split a 22.5° piece and pattern it 16 times.

If anyone out there is willing to do this with iLogic, I'd grant half of my part of the million: 45% =  (100% - 10% for Jeffrey)/2

[stephenmcd74]

Hello again Walter

This really is great stuff!!!

My ability with Inventor is not nearly as advanced as yours, so while this may all seem fairly obvious to you, for me it will take some time to get my head around it.

So as soon as I have time, I will sit down and try to work through your explanation, so see if I can replicate it myself.

Just to understand 1 thing please, Walter: On the gear you have sketches 4-18, and on the rack you have the 3d sketch. Am I right in thinking that these are both part of your first method, and therefore NOT part of the preferred solution #2? If so, is there anything else in there which is also part of solution #1, and therefore should be set aside by me when I am trying to work through solution #2?

Thanks again

Stephen

[WHolzwarth]

Ok. Let's move on to the next million.

Attached is a new fileset, only for 2nd method. (2015 files).

I just noticed Curtis watching here. IMO, iLogic would be no problem for him. We'll see ..