How do you turn a knurled part?

[stoltenkamp.scott]

Can anyone give me some guidance on how to turn knurls in Fusion CAM?

I've got straddle style knurling tools and bump knurl tools and use both.

I'm cutting multiple parts out of a single piece of stock.

I don't see any kind of option for a dwell when making contact with the part in either of the threading or grooving toolpaths, nor do I see a MasterCAM style "point" toolpath.

Attached is a very simple part with 2 knurled surfaces for representation.

I'd like to bump knurl the 1.5" diameter and feed along the 1" diameter.

Thanks for any help!

[Richard.stubley]

Hi @stoltenkamp.scott,

For the bump knurl I would use a single grooving pass and turn on the dwell before retract.

For the feed knurl I would then just use a traditional Finishing pass but make sure its starts on and off the job sufficiently, you may have the best results drawing a sketch line for this.

We haven't got a Knurling tool you can define in the library, I would define a grooving tool to show the same dimensions as your knurling tool. 

Hope this helps.

[stoltenkamp.scott]

Richard, I can't tell you how many dozens of times I overlooked that "Single Groove" toolpath. That's exactly what I was looking for regarding the bump knurling.

Do you happen to know a trick to allow grooving tools to be used in the finish toolpath? Every time I've tried it's always given me the following error:

Toolpath is not supported for the given tool and settings.

What setting am I overlooking, or is there a way to custom build a grooving tool that won't give that error?

[Richard.stubley · Accepted solution]

Ahh sorry I didn't realise it would allow that, serves me right for not checking first.

Ive got it to work quite nicely with the "Turning Groove" Strategy.

I made a sketch with the line I wanted the tool to follow, i wanted 0.2 clearance and I guessed a tool width of 1nch.

This line was then selected in the geometry tab.

Make sure you have roughing passes off.

Hopefully the resulting toolpath will be what your after.

[stoltenkamp.scott]

Richard.. thanks so much!

Instead of using the sketch method I just picked a point and used the toolpath front and back geometry with offsets to position the beginning and end of the toolpath. Seems to work well.

There is 1 little quirk though.. I'm getting a Feed command at the beginning of the second knurl toolpath that I don't think I'm defining anywhere.

it doesn't matter which order I put them in it shows up when I have both toolpaths back-to-back.

N196 G1 X2.3 Z0.1969 F0.66667

It's not a game breaker or anything, it just seems to come from out of nowhere.

[Richard.stubley]

Not a problem, glad its worked for you.

Regarding the feedrate, what post processor are you using?

[stoltenkamp.scott]

Post attached... dated January.. i think it's the current one, and I don't recall having tweaked it any since the last system refresh which was earlier this month.

That one feed command is a non issue for this project. I'm just kind of curious what spawned it.

[Richard.stubley]

I wont pretend to know 100% but we do some maths behind the scenes and assign "getHighFeedrate" for the G1 move if we are using feed per rev, if not then on line 37 we hard code it.

Line 37: highFeedrate = (unit == IN) ? 100 : 5000;

I know it wasnt essential but it's always nice to know what's happening when you are the one pushing cycle start.