Strutt Epicyclic Train Clock (maybe?)

[Jasonb]

That was what I was suggesting, use a 1mm (approx 0.040") cutter as they are readily available and being 7thou smaller than 3/64 might fit into the root of your gears.  Just enter the cutter diameter and the post processor will do the rest and set a tool path 0.020" from the edge. parts can still be in imperial.

Are they Cyclodial gears as those tend to be used more with the "Lantern" pinions that you describe, although Involute will work too.

[kvom]

I didn't understand the metric suggestion, and yes a metric cutter could be used.  The new mill uses ER collets and I suppose one of these would fit the shank.

But with closer attention to the photos in the book it is evident that the tooth form is epicyclic, so I'll need to regenerate in Gearotic and replace in SW before determining the tool needed to cut.  But Gearotic states that the maximum tool to cut the profile is .0471 and 3/64 is .0469.  Plus I still will need to scale to Smith's diameter adding a few thou to the width.

... some time later ...

Redone 66 tooth gear (called Sun Wheel in the book).

[internal_fire]

But with closer attention to the photos in the book it is evident that the tooth form is epicyclic, so I'll need to regenerate in Gearotic and replace in SW before determining the tool needed to cut.

Clock gears are virtually always "one-sided". The working side of the tooth should be made to match the design. The non-working side can be anything that looks OK. This provides a lot of flexibility for the choice of cutters.

Gene

[kvom]

I hadn't realized that.  But in this case my gear generator gives symmetric teeth.  I could have SW sheer off one side of each tooth, and even if I don't know yet which side is working I can always turn it around.   

[crueby]

No need to go to any trouble to cut back one side of each tooth. Remember that some will engage both sides while winding/setting the clock. If you take off extra on the off side, you run the risk of something jamming up during those times. Better to keep things properly symmetric.

[Jasonb]

With 7 thou to play with the 1mm cutter will allow a roughing cut and then final profile. Just make sure you have the minimum cutting radius set low for the roughing cut if doing it with an adaptive and use a larger one to take out the bulk of the material.

The cyclodial gear will also have a different overall diameter so that may be why you are seeing a difference between book and Gearotic. It will also be a bit wider at the root than an involute gear.

[kvom]

I plan to do the roughing pass with the 3/64" cutter on a ramped toolpath with .002" clearance and the finishing path full depth.  Feeds and speeds to be determined when I know the geometry of the endmill.  I don't plan to order any Chinese endmills.  Did that once, never again.

[internal_fire]

No need to go to any trouble to cut back one side of each tooth.

I was not suggesting that the gear should be purposely mis-cut. However, if an otherwise useful cutter would take off a few extra bits off the non-working side of each tooth it would not impact the operation of the clock. Talking about a few thousandths, not a large amount.

Any slight irregularity when winding or setting will almost certainly not matter.

Gene

[kvom]

I got the other wheels converted to cycloidal tooth form, but the largest wheel (called the ring wheel) has both internal and external teeth.  The external rim has 168 teeth, and the internal has 144.  Gearotic will generate only involute teeth for a planetary gear, so I'll have to use this.  (I suppose I could probably do cycloidal form manually in SW if absolutely necessary.  Smith had a homemade gadget to cut the interior teeth with the same cutter.  I wonder how other builders will do or have done this.

I had to generate this as separate gears for the inside and outside to get the tooth forms in DXF format.  However, it does not appear possible to insert two DXF files into the same part, nor cut/paste from different parts.  So my eventual solution is to generate two separate rings and mate them into an assembly.

[Jasonb]

You should just be able to copy the profile of the gap between two external teeth, paste that over the inner edge and cut, then do a circular pattern. Unlike involute gear cutters the Involute cutters will do a large range of tooth counts with only the very smallest pinions needing a specific cutter.

I have selected and copied parts of a DXF and DRG files and imported into my 3D model  in Alibre, Solidworks should have a similar facility. See this post as an example

https://www.model-engineer.co.uk/forums/topic/turbocad-question-accurate-printing/#post-699125

[kvom]

I had a struggle with this as SW got into a never-ending loop trying to replicate the tooth-form splines 144 times.  I generated the gear with the external teeth, copied one and mirrored it, then ensured that the completed single tooth form covered exactly 2.5 degrees of the circle.  The mirrored teeth will be slightly closer together than the external version. 

[crueby]

Bet that burnned up a big box of electrons!

Question: are there the same number of teeth on the inside set? Not going to count them! For the same size tooth, the inner set would have to be a lower tooth count? To my eye, the gaps on the inner ones look to be smaller than on the outer ones, but that could just be an optical delusion. The gaps on the inner ones just need to be wider than the wire size used on the lantern pinion, at the base as well as where they start to curve near the ends where they are closest together.
Chris

[petertha]

Some progress and some frustration with SolidWorks.  The progress was in figuring how to trace an image to generate the plates.  The answer is to scan the drawing in the plan book to a BMP file, and then use the Insert Sketch Image into the open sketch.  Then I was able to do the points/splines and circles on one half, then mirror it to get the entire plate.  The result was over 5 times the needed size, but I could measure the paper sketch to obtain the scale factor, and then scale the SW sketch.

Just a few FYI's. The source image can be any of the common formats, JPEG etc. (not just BMP). Perhaps you missed a feature step where you can 'scale' the image to some convenient known dimension on the image using the blue line start/end points. It can be from anywhere to anywhere, not necessarily orthogonal. This is best done early in the modelling tracing exercise, not later. Look for an important dominant dimension or a relatively large span of known length, click the image points & enter the value directly. The image shrinks/grows accordingly & now you are more in tune with the actual modelling. Of course this does not correct image distortion issues, its a good start.

https://help.solidworks.com/2025/english/SWConnected/swdotworks/t_insert_and_resize_pictures.htm

There is also a semi-automated way SW can generate outline splines if the source image has decent contrast &resolution. Usually its a recipe for disaster on any kind of mechanical image because it will inevitably guess wrong, but the capability does it does have its place. My friend sent me a snapshot of rather complicated decal on a car hood he wanted a DXF file to use for subsequent cutting. The auto-trace did a great job on 95% of it, I just had to do some minor cleanup which was a lot easier than developing every sketch element from scratch. This video touched on both these concepts but there are other tutorial on the interweb.

<a href="https://www.youtube.com/watch?v=TL_dkhFncUo" target="_blank">http://www.youtube.com/watch?v=TL_dkhFncUo</a>

[petertha]

I had a struggle with this as SW got into a never-ending loop trying to replicate the tooth-form splines 144 times.  I generated the gear with the external teeth, copied one and mirrored it, then ensured that the completed single tooth form covered exactly 2.5 degrees of the circle.  The mirrored teeth will be slightly closer together than the external version.

Unless I'm missing a key aspect of the design, I would go about this differently. Generate the single tooth A using your tooth sketch, extrude that however it needs to be extruded. Then use the circular pattern command & define how many instances (teeth). Boom, done. Repeat for inner tooth B which allows for a different tooth sketch form & count as required. This is the power of parametric design. If you later need to modify the tooth form, you just alter the single sketch which defines it, then all the downstream steps magically refreshes & updates. Same goes for altering tooth count (or angle between, they are related) just enter a different integer.

[Jasonb]

I had a struggle with this as SW got into a never-ending loop trying to replicate the tooth-form splines 144 times.  I generated the gear with the external teeth, copied one and mirrored it, then ensured that the completed single tooth form covered exactly 2.5 degrees of the circle.  The mirrored teeth will be slightly closer together than the external version.

It is not the tooth you need to copy. it is the gap between as that represents what a cutter would remove. Then as I said cut one "gap" with that sketch and do the circular pattern of 144 letting the CAD work out the angles, tooth thickness etc.

This way the gaps stay correct and will fit the wires of the lanturn pinion