Hobbing contrate/frontal teeth

[stephenmcd74]

Good afternoon everyone

I wanted to model some contrate teeth which have been hobbed/generated.

Outer radius of hobbing cutter is 6mm.

I modelled the cutter, and  then implanted this 20 times in an assembly which contains the pinion to be hobbed. The aim is to break down the continuous process of hobbing into 20 steps for a half of a single tooth space. This could then be mirrored to create a single tooth, albeit with slightly jagged areas because of the 20 steps.

From within the assembly, I edited the pinion and used copy object to bring the 20 cutters into the pinion part file. I had hoped to use combine to then cut away the material where the cutters intersect with  the pinion. This could be done by either combining the cutters into a single larger object, and then subtracting this from the pinion (the combining didn't work at all - WHY??). Or, individually subtracting each cutter form the pinion using combine: this also didn't work, as combine fails after a maximum of 4 combines.

Alternatively, in the assembly I edited the pinion, and drew a new sketch on the tangential face of the cutter, which gives me the profile of the cutter. I then drew a second sketch at right angles to, and through the centre of, the first sketch, and drew an arc of r=6mm from the tip of the cutter to use a a guide. So I then used Sweep to move the profile in the first sketch along the arc in the second. This worked once, but failed on the second (out of 20!!) cutter.

Can anyone see a way to get this to work, or even see a better way of solving the problem?

Some files are attached

Many thanks

Stephen

[WHolzwarth]

Stephen, I'm late, but I think, there's an error in the general approach.

At first, let me ask:

- You want to create 12 teeth. Is that ok?

- The workpiece is rotating steadily without stops. Ok?

- Now hobbing. I know of a minimum of two methods for normal teeth:
a)  Cutter is proceeding axially, and rotates together with the workpiece

b) Workpiece is quiet. Cutter moves axially, and is set back after the cut. Then workpiece will rotate 360° divided by number of teeth. Same procedure for the next tooth.

But here, the cutter axis is not parallel, it's perpendicular. What's going on? Can you show a drawing or a picture of the cutter?

I'm asking that, because there needs to be an intermediate period with no contact between workpiece and cutter.

[stephenmcd74]

Hello there Walter

Very nice to hear from you again, and thanks for taking a look at this.

In answer to your questions:

• pinion has 16 teeth
• Yes, during the hobbing process, the workpiece (pinion) rotates at a constant speed, without any stops
• Hobbing proceeds as you describe in a)

But Walter, these are not conventional 2d hobbed gear teeth like the ones you looked at before for me. These are frontal/contrate hobbed teeth. I have done an assembly showing the machining process - see attached. It shows the actual machining arrangement for the pinion and the cutter as they would appear on the hobbing machine. Note that the cutter only has 3 teeth (2 complete turns of the helix). So if the pinion was rotating about its axis at 1 rps (revolution per second), the cutter would be rotating about its respective axis at 16 rps.

Please note also that the pinion attached ("pinion 16 teeth hobbed") was modelled by using the old technique of placing the cutter in the pinion at the first, last, and 1 intermediate position in order to create 1 side of s single tooth space, and subtracting these from the pinion. I then mirrored this to create a complete space, and patterned it x16 to create the rest of the teeth. So the profile of the teeth in this pinion is precise, except that it has various jagged edges because of only 3 passes of the cutter for each half-space. My aim here is to try to find a way of creating this same geometry, but by sweeping the cutter through the pinion, in order to create geometry which is both accurate and smooth - effectively just like the result you would get from actually hobbing these teeth on a machine.

Does that make things any clearer?

Many thanks for your help

Stephen

[WHolzwarth]

Hmm. Would this be a usable shape for the tool? Is it a grinding process?

[stephenmcd74]

Hey Walter

Your tool is slightly too wide. I have redone the version I sent you before, but completed the cutter. Please have a look at the revised files attached.

No it would be a normal cutting process - not grinding - so you have to imagine that the cutter has teeth - no different from a normal hob, except for the fact that there are only 3 complete turns of the helix.

Stephen

[stephenmcd74]

Please see files attached.

I had hoped to model it in this way: so the pinion effectively stays still, and a single tooth of the cutter is swept in such a way as to replicate the compound motion of both the rotation of the pinion and the translation of the cutter together. The starting point of the cutter would be SC Z3 R6 #1 in that assembly, and its finishing point would be #21. 

The path (an interpolated spline) is found in sketch 17 of "BWC2-2003-1 for hobbing2"  - please see above where I have described the red spline.

Could this work?

[johnsonshiue]

Hi Stephen,

I took a look at the latest part you attached last night. With the spline path, the Solid Sweep did not work. I think you will need to simplify the path to a few arcs. Is it possible? Does it have to be a spline?

Many thanks!

[WHolzwarth]

That's what I got with 2020 Solid sweep. Some tricks were needed.

[WHolzwarth]

Now with a chamfer at the inner edges of the teeth.

[stephenmcd74]

Walter

Sorry but I don't think you are there yet.

Attached is that pinion I already mentioned which I modeled using just 3 passes of the cutter (first, last, and one in the middle) for one side of a single tooth space. The tooth profile is jagged, but accurate I think.

Put this in an assembly with your 2 pinions and constrain them all on top of each other. You will see the differences.

I can only suggest you look again at sketch 17 of "BWC2-2001-3 for hobbing2", which shows you the geometry required to move the cutter from 1 tooth space to the next. and how this geometry is generated for M=0.122 and Z=16.

Or are you trying this some completely different way?

Stephen

[WHolzwarth]

Next one, and enough for today 😴

[karthur1]

Walt,

I tried to use his spline curve for the solid sweep and like you, it failed on me.  Wondering if you would post the actual .ipt file so that I could see what trick that you used to make the sweep happen.

Thanks

Kirk

[WHolzwarth]

Solid sweep is not mature enough yet, Kirk. Under some conditions it's working, in very similar situations it doesn't.

Here's the 2020 file. I didn't check it again for included unsuccessful attempts, but the result should do.

Short time later:

Oh, an error. In Sketch18 the angle should be set to 11.25° instead of 12.25°.

[stephenmcd74]

Good morning Walter

Sorry not to have replied yesterday - been completely tied up with other stuff.

Ok so could I run a few points past you please:

• Did you check your pinion against mine ("pinion 16 teeth hobbed"), by constraining them together in an assembly, so that you can clearly see the differences? If so you can see that there are still significant differences, although, of course, everything is lovely and smooth on yours. Is this the closest you can get?
• Unfortunately I still have Inventor 2015, so can't open your ipt file. I understand that it wasn't possible to use my interpolated spline as the path for the sweep, and yes, that would seem to be a great pity. But please could you describe your alternative method?

Thanks

Stephen

[stephenmcd74]

Hi Johnson and Walter

My original method was similar to what you proposed, Walter, back in 2016 for the 2d hobbed teeth. I placed 21x the cutter inside an assembly with the pinion (please see files attached), and used copy object to copy all of the cutters into the pinion ipt (this only worked if I copy them one by one). I then wanted to use combine to subtract the cutters from the pinion, with the logic being that the higher the number of instances of the cutter, the smoother the result will be.

However, this doesn't work at all, because combine will only let me utilise a maximum of 3 of the cutters . any more and it fails. So the result is "pinion 16 teeth hobbed", which is very jagged, but accurate.

Can someone explain why this doesn't work, of if there is a way to get this to work?

Thanks

Stephen

[WHolzwarth]

Hi Stephen,

is your part only an idea, or has it been manufactured already in this shape?

Normally for 16 teeth, there's an angle from tooth to tooth as 22.5°. I think, the relative angle between tool and workpiece can't be greater than this value, 11.25° to both sides versus a midplane of the tooth.

At the moment, I don't see a setup for a continuous rotation of the workpiece for bigger gap angles than 22.5°.

I think, your part can only be done this way:

- Workpiece stop

- Linear proceed of the tool along the main axis (vertical)

- Swiveling from left to right (2 x 22.5°)

- Tool moves back, vertical

- Workpiece rotates 22.5° to next tooth, and stops

- ...

[WHolzwarth]

Oh! I see, there's more possible. I've created a cutter with blades and placed it versus my existing part. With a collision analysis it's obvious, that a wider cut can be done.

[WHolzwarth]

Here's a new part. It's still not perfect, because the helix angle of the hobbing screw is neglected. But the videop shows, what's going on.

[stephenmcd74]

Hi Walter 

That looks great - I think you are really on the right track now!!
Please can I ask you to explain to me how you have done this (sorry but I am still on Inventor 2015)?

Thanks

Stephen

[stephenmcd74]

Hello again Walter

I realise that the world has changed completely since we started this discussion, so maybe it is no longer possible for you to be at work?

Anyway, if you read this message, and if you have an opportunity to respond then brilliant. If not then no worries.

I was interested in your progress on those teeth which you "hobbed". Unfortunately I am still on Inventor 2015, so can't open your .ipt file to see how you did it. Could I please ask you to explain your method? Is it using Sweep Solid, or a completely different approach? Also, you mentioned before that Sweep Solid didn't allow you to select the spline which I had drawn as the path, so is your method an accurate representation of these hobbed teeth, or a close approximation? If an approximation, on what did you base it?

Thanks for your help, and I hope that all is well with you.

Take care

Stephen

[WHolzwarth]

Stephen, I'm hoping, to be still in good health. But it's only the situation right now, nobody knows the future.

This hobbing can be done by solid sweep, but it's not really needed. See picture.

The cutting solid can be created by patterning two end solids, and filling the gap between them with revolve surfaces.