[tkms002]

No way of knowing. You're cutting MDF on ... is it a CNC router table? Not sure what cutter you're using. If you're able to cut 60"/min in a straight line without any issues, then you "might" need to just slow it down a bit for profiling the insides of those slots. That's a tight corner to make if you look at what the centerline of the cutter has to do to make that corner.

I'm sure you have a lot more experience with MDF than I do, so you will have a good "feel" for how fast you can cut it. I'm thinking more about what your machine has to go through to make a tight arc/circle at high feed rates. :-)

PM

yes, A DIY CNC Router table.
I have manual router experience but I have no idea how fast I am pushing it. As you said, it is by feel.

[tkms002]

The reason it's not boring all the way through is because you have Stock To Leave set at 0.02". Turn that off and it goes all the way through. Not sure on the plunge outside of stock message, only had a minute to look.

David

I dont get it. I have opened both the files I sent you and I dont see STOCK TO LEAVE turned on in either one. When I do click that box it shows .004.
Attachment 419696

[difalkner]

I dont get it. I have opened both the files I sent you and I dont see STOCK TO LEAVE turned on in either one. When I do click that box it shows .004.
Attachment 419696

I just downloaded your file in Post #12 again and opened it to the Passes Tab. It shows Stock To Leave set at 0.02".



David

[tkms002]

I just downloaded your file in Post #12 again and opened it to the Passes Tab. It shows Stock To Leave set at 0.02".



David

but I have not run that tool path. I ran the first tool path. The profile pass to cut out the part and it does not have the stock to leave checked but still only goes .475 deep.
Attachment 419706

Also, in the generated G-code I see several places where .475 is listed. What are they doing?
g-code is attached.

[tkms002]

ok My bad. I must have run a different program.
I re programmed one just now and it cut all the way through. I made sure I did not have stock to leave checked.

Thanks

[tkms002]

when I ran my last program I first removed the beginning g28 and the line with M6 in it.
After the cut was complete it sliced an angle through the part as it was going back to my home. I am assuming this was because of the last G28 in the code?
Code is here
%
(1001)
(T1 D=0.25 CR=0 - ZMIN=-0.5 - flat end mill)
G90 G94
G17
G20
G90

(2D Contour4)
M9
S24000 M3
G54
M8
G0 X-3.692 Y-4.875
Z0.6
Z0.2894
G1 Z-0.25 F13.12
X-2.625 F60
G3 X-2.5 Y-4.75 J0.125
G1 Y-3.25
G3 X-2.625 Y-3.125 I-0.125
G1 X-3.692
G2 X-4.0167 Y-2.9375 J0.375
G3 X-4.125 Y-2.875 I-0.1083 J-0.0625
G1 X-7.125
G2 X-7.5 Y-2.5 J0.375
G1 Y-1.25
G2 X-7.125 Y-0.875 I0.375
G1 X-0.875
G2 X-0.5 Y-1.25 J-0.375
G1 Y-6.75
G2 X-0.875 Y-7.125 I-0.375
G1 X-7.125
G2 X-7.5 Y-6.75 J0.375
G1 Y-5.5
G2 X-7.125 Y-5.125 I0.375
G1 X-4.125
G3 X-4.0167 Y-5.0625 J0.125
G2 X-3.692 Y-4.875 I0.3248 J-0.1875
G0 Z0.2
Y-3.125
G1 Z0.0394 F13.12
Z-0.5
G2 X-4.0167 Y-2.9375 J0.375 F60
G3 X-4.125 Y-2.875 I-0.1083 J-0.0625
G1 X-7.125
G2 X-7.5 Y-2.5 J0.375
G1 Y-1.25
G2 X-7.125 Y-0.875 I0.375
G1 X-4.3
X-4.25 F15
X-4.1697 Z-0.4599 F60
X-4.125 Z-0.4375 F15
X-3.875 F60
X-3.75 Z-0.5 F13.12
X-0.875 F60
G2 X-0.5 Y-1.25 J-0.375
G1 Y-3.7
Y-3.75 F15
Y-3.8303 Z-0.4599 F60
Y-3.875 Z-0.4375 F15
Y-4.125 F60
Y-4.25 Z-0.5 F13.12
Y-6.75 F60
G2 X-0.875 Y-7.125 I-0.375
G1 X-3.7
X-3.75 F15
X-3.8303 Z-0.4599 F60
X-3.875 Z-0.4375 F15
X-4.125 F60
X-4.25 Z-0.5 F13.12
X-7.125 F60
G2 X-7.5 Y-6.75 J0.375
G1 Y-5.5
G2 X-7.125 Y-5.125 I0.375
G1 X-4.125
G3 X-4.0167 Y-5.0625 J0.125
G2 X-3.692 Y-4.875 I0.3248 J-0.1875
G1 X-2.625
G3 X-2.5 Y-4.75 J0.125
G1 Y-3.25
G3 X-2.625 Y-3.125 I-0.125
G1 X-3.692
G0 Z0.6 is this the retract height before the rapid to home? stock is only .5 thick
M9
G28 G91 Z0
G90
G28 G91 X0 Y0
G90
M30
%

Attached it the fusion file

here is a pic of the damage
Attachment 419718

how do I keep that from happening?

Thanks

[difalkner]

Got it what speed would you suggest for the slots and the holes?
Thanks

I regularly cut 1/2" Baltic Birch with a 1/4" compression bit running 18k rpm, plunge to 0.25" depth of cut, and typical feed rate of 175 ipm - no issues at all. Just cut a Longworth chuck an hour ago using these settings. I cut the center hole, finger holes, slots, and outer profile at the same setting.

Attachment 419720

David

[Jim Dawson]

when I ran my last program I first removed the beginning g28 and the line with M6 in it.
After the cut was complete it sliced an angle through the part as it was going back to my home. I am assuming this was because of the last G28 in the code?
Code is here
%
(1001)
......................................

.....................................
G1 X-3.692
G0 Z0.6 is this the retract height before the rapid to home? stock is only .5 thick
M9
G28 G91 Z0
G90
G28 G91 X0 Y0
G90
M30
%


how do I keep that from happening?

Thanks

Try this, set G28 Safe Retracts = No :


Then run an air cut and see if it fixed the problem.