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Modelling gear hobbing 'exit' in Solidworks?

Beauvais

Aluminum
Joined
May 15, 2022
I'm trying to model a helical gear on a shaft but cant create the gear cutter exiting the shaft. I've found a video of someone doing this in Solid Edge but SW seems to have no option to do this..

Anyone have any idea?

Screenshot 2024-04-14 160719.png



Screenshot 2024-04-14 161658.png
 
This would work in wildfire and since saladwurx is just a copy of pro/e -- take the shape of the tooth space at the end of the gear's travel. Sweep it on an arc the radius of the hob (most common hob size for what looks like your part would be 3" diameter) along the helix of your teeth.

This isn't going to be totally exact because the movements of all the parts are a bit more complicated than that, but it'll be close enough for government work. The tooth shape is pointless in a solid model anyhow, it's just for looks.

p.s. the technical term is 'runout'. Yeah I know, sounds like the shaft is bent but in this case, just means the area where the hob runs out of the part.
 
Unfortunately in revolved cut it cant follow the helix, and swept cut it will only follow either the helix or a sketch path following the cutting path and runout :( It wont let you use 'guide curves' to follow the helix.
 
Not sure about SolidWorks specifically, but my general approach would be to draw a planar sketch curve for the sweep to follow consisting of a straight line along the cylinder (for the full-profile tooth) and an arc (for the runout). Sweep the involute profile along this planar curve. Then twist the resulting solid around the axis of the shaft. This might be called "Flex" in SolidWorks, but I'm not sure. Finally array the result around the shaft axis to get your 10 grooves and boolean subtract these 10 cutters from the cylindrical shaft to get the gear.
 
Unfortunately in revolved cut it cant follow the helix, and swept cut it will only follow either the helix or a sketch path following the cutting path and runout :( It wont let you use 'guide curves' to follow the helix.
Have done this in Pro/E (slowly, practice makes perfect and it isn't something I do every day) so I'd be shocked if saladwurx can't do the same thing. Example - just switch from extrusion to a cut :

swept.jpg

some pointers about the technique



and this isn't exactly what you need but might point you in a better direction, it's a bit similar but using your fave cad program instead of mine :)


this guy is pretty good, but again, pro/e ...

 
174479827.png
 
David_M said:
Showoff :D

Looks nice, actually. Did you just throw a construction plane up at the helix angle where the teeth ended, then drop an arc on that ? I was thinking that'd probably be plenty good for this.

You're supposed to teach a man to fish, ya know ...

Here, let me make myself useful for web searches -- "modelling hob runout"
 
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EG,
I think I can think of a couple of ways to do it using my Rhino. The one above I did quickly by taking one tooth space and having it follow a guideline ending with a radius similar to what I imagine the hob's to be. After that, array the tooth space into a complete spur gear. Then, twist it into a helical. You do need to give it a new OD after the array operation to fill in the extra area caused by the cutter's incomplete cutting of the gear spaces.
 
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Creating a 'straight' profile of the runout then using flex would work.. In other programs perhaps but sw likes to make things out of round when you flex unfortunately so you cant even make a purely visual gear as you cant then extrude the same diameter.

Solid Edge will do it without fuss but I'm determined to do it sw. @EmGo I think this is the best bet, creating a 3d sketch curve of the runout path, I'm just stuck trying to figure it out at the minute.
 
Have to admit, I love it when someone else is just as pigheaded stubborn as me :D

I could be kind of mean and ask if you are going to model the tip relief on that part as well :)

I've been thinking about the steps to do it in solid edge, using the same helical cutout feature.. I'm just finishing up the other parts first otherwise I'll lose motivation lol, its a steering rack pinion if you're interested.

Screenshot 2024-04-13 140209.png
 
Is it possible to twist a sketch in SolidWorks? If so, I'd draw a planar line+runout curve (blue) and twist the curve around the axis of the cylinder to get what's shown in magenta. I've exagerated the twist.

Then use the magenta curve as the guide for a sweep. But, the right orientation rule needs to be used when sweeping. It looks like that might be called "Direction Vector" in SolidWorks. Use the axis of the cylinder as the direction vector.
 

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Use the axis of the cylinder as the direction vector.
Don't know how solidwurx does this but will mention - the shape of the tooth space has to be at right angles to the helix. In fact if one were contour milling these teeth I'd be concerned about the shape just being twisted, not sure what you are really getting that way, but for artistic purposes it's plenty good.
 
You can append a sketched sweep-out radius to the original helical curve using the "Composite Curve Command", which assuming you are using a swept cut, can give you something that is at least visually similar to the actual hobbed runout (see attached screenshot). When I modelled this I had to specify a profile twist value to get the sketch to rotate properly along the path during the helix, but that same profile twist may be distorting the runout geometry (Note this model isn't a "real" gear, I just threw it together to look like a gear for demo purposes). You could also probably model the runout as a separate swept (or revolved) cut after the initial helical sweep, which should accurately model the as-machined geometry without fussing with profile twists. But I have to wonder why one would bother with this detail.

Screenshot 2024-04-15 143220.png

However you choose to model these features in CAD, like others have said, I would discourage you from modelling the teeth at all, since it bogs down your system and accurately modelling the feature doesn't add any value unless you are printing the part. It's like modelling threads on screws, another detail which most engineering companies actively discourage.

In theory you could also model this geometry using a solid sweep command, and should get exactly the hobbed geometry. However solid sweeps within Solidworks are super slow and computation intensive even when they work, and in my experience they rarely work (either they crash SW or generate bogus wavy geometry that doesn't reflect reality, which is what happened in this case when I tried it, see the following screeenshot)Screenshot 2024-04-15 144222.png
 
You can append a sketched sweep-out radius to the original helical curve using the "Composite Curve Command", which assuming you are using a swept cut, can give you something that is at least visually similar to the actual hobbed runout (see attached screenshot). When I modelled this I had to specify a profile twist value to get the sketch to rotate properly along the path during the helix, but that same profile twist may be distorting the runout geometry (Note this model isn't a "real" gear, I just threw it together to look like a gear for demo purposes). You could also probably model the runout as a separate swept (or revolved) cut after the initial helical sweep, which should accurately model the as-machined geometry without fussing with profile twists. But I have to wonder why one would bother with this detail.

View attachment 436278

However you choose to model these features in CAD, like others have said, I would discourage you from modelling the teeth at all, since it bogs down your system and accurately modelling the feature doesn't add any value unless you are printing the part. It's like modelling threads on screws, another detail which most engineering companies actively discourage.

In theory you could also model this geometry using a solid sweep command, and should get exactly the hobbed geometry. However solid sweeps within Solidworks are super slow and computation intensive even when they work, and in my experience they rarely work (either they crash SW or generate bogus wavy geometry that doesn't reflect reality, which is what happened in this case when I tried it, see the following screeenshot)View attachment 436281


Thanks for this! Could you show me the feature tree when you used the composite curved command? I dont know how I need the runout sketch to join the helix.
 
You just need the runout sketch end to be coincident with and tangent to the end of the helix. I did this with a bunch of planes, points and axes because I was messing around. If this were a model for anything other than a demo I would take the time to model it more efficiently. Note the runout transition isn't normal to the helical path in this model, so it's not technically the correct runout. See below:

1713220668600.png

If you model the runout as a separate swept cut from the helical groove, you can make the runout sweep path as a plane normal to the end of the helical swept cut, and intersecting a radial line at the end of the swept cut (assuming you model the tooth space correctly, as normal to the helical path, rather than parallel to the end face of the gear. In your initial model at the start of this thread you made the cut sketch parallel to the end face of the gear). Note in this model the runout to helical transition is normal to the helical path, which is nearly the correct, actual geometry (except for minor profile differences since the hobbed runout will be a different tooth profile than this sweep will model). But once again I can't see why anyone would care if you modelled the gear correctly to this level of detail. See below:

1713222233563.png

This took longer than I wanted to spend on it and I'm not sure I'll ever use it myself, but here we are.
 
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You just need the runout sketch end to be coincident with and tangent to the end of the helix. I did this with a bunch of planes, points and axes because I was messing around. If this were a model for anything other than a demo I would take the time to model it more efficiently. Note the runout transition isn't normal to the helical path in this model, so it's not technically the correct runout. See below:

View attachment 436285

If you model the runout as a separate swept cut from the helical groove, you can make the runout sweep path as a plane normal to the end of the helical swept cut, and intersecting a radial line at the end of the swept cut (assuming you model the tooth space correctly, as normal to the helical path, rather than parallel to the end face of the gear. In your initial model at the start of this thread you made the cut sketch parallel to the end face of the gear). Note in this model the runout to helical transition is normal to the helical path, which is nearly the correct, actual geometry (except for minor profile differences since the hobbed runout will be a different tooth profile than this sweep will model). But once again I can't see why anyone would care if you modelled the gear correctly to this level of detail. See below:

View attachment 436287

This took longer than I wanted to spend on it and I'm not sure I'll ever use it myself, but here we are.

Thank you! Got there in the end lol.

Screenshot 2024-04-16 015230.png
 








 
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