Parting off cylindrical part

[vich...@gmail.com]

I would like to know what CAM operations to use when parting off a cylindrical part. Here is a simple example.   https://a360.co/2O6nML3

When you click on the link, this will show the part. The small diameter on the part is the area to part off.

Thanks Vic

[Graham Stabler]

I typically just use a 2D contour and cut from one side if my tool will reach, for plastic parts I will pull lightly to make them hinge when it gets thin to prevent marking. If you want a perfect result then leave some material and machine a little fixture to hold it for a second operation.

An alternative is to use a wrapped tool path more like you were using a lathe but they don't work if the path is a circle, you can split a circle into two though, just leave out leads in/out and keep the tool down etc.

Cheers,

Graham

[Brad Cavallaro]

Hi all, 

I understand the logic of the above answer, but in the spiral part provided by Pocket NC, it's clear that cutting off the cylindrical part is possible by moving z in as b spins. Can someone explain how it was done in Fusion, or provide the fusion model. Upload the attached file to the pocket NC simulator to see how the cut is done. https://sim.pocketnc.com/

Find Spiral tool path here https://pocketnc.atlassian.net/wiki/spaces/PNFUR/pages/370507881/Pocket+NC+V2+Demo+Part-Spiral

[azdavi...@gmail.com]

Its not letting me post that code as a file but just open up notepad or notepad++ and save it as a .ngc file.

[azdavi...@gmail.com]

Many of the fusion machining operations are not capable of processing what they call "cyclic" profiles or surfaces, but you can break up cyclic surfaces and then machine them. in the case of the spiral shown it can be done using the wrapped tool path. and isn't cyclic. An alternative to the manual code I posted above is doing a swarf tool path on a flat disk with the center cut out, set the inner edge as the bottom and the outer edge as the top, and then have it "spiral down". the drawbacks are the tool path it makes will be crappy and not smooth at all, additionally you cant go past the center, however it can be down off center, and the parameters controlled in fusion more easily.

All this being said  I dont part off my parts like this, I use and endmill and mill a slot using a ramped tool path from 3 sides leaving 3 little legs to break off, this prevents my part from getting chucked off.

[azdavi...@gmail.com]

Fixed a few things, fusion doesnt like commas haha:

 Basically the best way to do this in fusion is to add in a manual pass through gcode operation. first you need to enable this by editing the pocket nc post, there is a guide of how to do this somewhere on the autodesk site. Once you enable it, add a manual gcode operation at the end of your list of ops. You can also just run this gcode on its own, but its nice to have everything in one place. you can run it in the simulator and see what it does as well, I tried to define what all of the codes actually do, some are redundant.

(Part off code)

G20 (G20: Specifies the inch is to be used)

G90 G94 G40 G17 (g90:Absolute programming G94:Feed per minute G40:Tool nose radius comp canceled G17:XY plane selected)

M0 (M0:manual pause in case you need to change tools or whatever)

M6 T1(M6: Select tool the t value is the tool you intend to use)

M3 S10000 (M3: turns the spindle on clockwise and the s parameter is the rpm)

G53 G0 Z0 (Z value here brings the tool all the way back away from the part to avoid collsion)

G53 G0 A0. B0.(G53: this is the machine coordinate system no offsets applied G0 is the rapid movement the values here a and b orient the rotary axis's properly for the part off)

G53 G0 X0.030 Y0.500(x value is your tool centerline offset this allows the endmill to cut more efficiently since there is minimal chip clearance in the center of the endmill y value is the part off height)

G43 Z0.5 H1 F40(G43: enables tool length compensation z value here is slightly above half the diameter of the stock IMPORTANT: H value is the tool to be used F value is the feed rate)

G43 B9540 Z-0.030 H1 F10(B value is the number of degrees to turn so in this case I want to do 0.020 axial depth of cut so I divide the depth to be traveled by the depth of cut and multiply by 360 the z value is the ending depth of the endmill H value is tool to be used)

G49 (G49 disables the tool length compensation)

G53 G0 Z0. (This line simply retracts the tool all the way back)

M5 (M5: Stops the spindle)

G53 G0 X2.5 Y2.5 (This line sends the x and y axis all the way back)

G53 G0 A0. (as the pocket nc has to rewind the b axis fully I suggest not sending the b axis to 0 stop the program after this line then home the b axis manually huge time saver)

M30 (M30 ends the program and returns to the start)

[azdavi...@gmail.com]

https://knowledge.autodesk.com/support/autodesk-hsm/learn-explore/caas/sfdcarticles/sfdcarticles/How-to-use-Manual-NC-options-to-manually-add-code-with-Fusion-360-HSM-CAM.html

[qrot...@pocketnc.com]

Hi all,

The demo Spiral Part that we provide is parted off with a Swarf operation. As David already mentioned, this does the trick but does not always leave a great finish. If the bottom of the part needs to have a nice finish we definitely recommend one of the other methods mentioned above. 

Happy machining! 

Q Rothing 

Applications Engineer, Pocket NC