Compression bit and cutting strategy in Cut2D

Post general information and questions relating to Cut2D in this Forum.

Compression bit and cutting strategy in Cut2D

Postby CX15 » Fri Jun 29, 2018 1:35 am

Hi Everyone
I'm still learning, so please excuse if I'm asking dumb questions...

I'm using a 1/8" compression bit. Details here: https://www.amanatool.com/46180-k-cnc-solid-carbide-spektratm-extreme-tool-life-coated-compression-spiral-1-8-dia-x-13-16-inch-x-1-8-shank.html
The switchover from downcut and upcut is 7/32 form the bottom of the bit.
I'm cutting (Baltic Birch) plywood of 1/2" thickness.
I'm initially working on making 4 cuts of 1/8" at a time (4th cut will be slightly deeper to cut through the wood).

My problem is that when making the first and second cut, the upcut portion of the bit is ruining the top edge of the wood.
Only at the 3rd and 4th cut is the compression working as designed (downcut at top edge and upcut at bottom edge).

So my question is basically how to work around this:

SCENARIO A: PROFILE CUTTING
I think have an working strategy here:
- In the 2D Profile Toolpath options, I select <Allowance offset> to 0.1"
- Then I select <Do Seperate Last Pass> with 0.0" Allowance

Does this make sense to do it this way?

SCENARIO B: POCKET TOOLPATH
Here I dont really know what to do.
I cannot see any options for an offset pocket followed by a final pass.
Any ideas will be greatly appreciated.


Let me know if I should make this clearer with some pictures or specific examples.
Regards
Andre
CX15
 
Posts: 6
Joined: Sun Apr 15, 2018 5:13 am
Model of CNC Machine: 6040Z

Re: Compression bit and cutting strategy in Cut2D

Postby mtylerfl » Fri Jun 29, 2018 2:54 am

Have you tried lead-in ramp cuts? You should be able to avoid ruining your top surface by allowing the bit to go to the appropriate depth prior to getting to the cut for the “good” portion of the material cutout.
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 3162
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Compression bit and cutting strategy in Cut2D

Postby IslaWW » Fri Jun 29, 2018 3:27 am

Your pass depths need to be deeper than the upspiral portion of the bit. 1/4" or more. In most cases compression bits are made to cut material in a single pass. Many smaller machines are not rigid enough to accomplish this accurately. If your machine cannot handle cutting the material in 2 passes, then you will have to use a different bit
Gary Campbell
CNC Technology & Training
The Ultimate Woodworking Machine
GCnC411 (at) gmail.com
User avatar
IslaWW
Vectric Wizard
 
Posts: 1078
Joined: Wed Nov 21, 2007 11:42 pm
Location: Marquette, MI, USA
Model of CNC Machine: The Ultimate Woodworking Machine

Re: Compression bit and cutting strategy in Cut2D

Postby CX15 » Fri Jun 29, 2018 5:14 am

IslaWW wrote:
mtylerfl wrote:Have you tried lead-in ramp cuts? You should be able to avoid ruining your top surface by allowing the bit to go to the appropriate depth prior to getting to the cut for the “good” portion of the material cutout.


Yes, I use lead-in ramps on all cuts, but this still does not resolve the problem.
If the first cut leads in to a depth of 1/8" , I'm still upcutting the top edge.

IslaWW wrote:Your pass depths need to be deeper than the upspiral portion of the bit. 1/4" or more. In most cases compression bits are made to cut material in a single pass. Many smaller machines are not rigid enough to accomplish this accurately. If your machine cannot handle cutting the material in 2 passes, then you will have to use a different bit


Thanks Isla, this actually makes sense to me. I just wasnt sure if the 1/8" bit would handle a single pass through 1/4" plywood. But I guess what you are saying is that it was designed that way.
I will give it a shot and see how the machine handles it.
CX15
 
Posts: 6
Joined: Sun Apr 15, 2018 5:13 am
Model of CNC Machine: 6040Z

Re: Compression bit and cutting strategy in Cut2D

Postby mtylerfl » Fri Jun 29, 2018 1:09 pm

Yes, that is what I was referring to also. You gotta get that bit to proper depth before it starts cutting the “good part” of the material so the upcut portion of the bit isn’t “ripping up” the top of it.

For 0.5” thick material, it shouldn’t be a problem cutting full-depth anyway. I cut up to 0.75”-thick Pine and Poplar at full-depth on the CarveWright CNC when using a 0.125” dia. EM. Hardwoods do require shallower pass depths...I’ll set pass depths at 0.3” or 0.4” on the CarveWright. I’ve broken only two 0.125” dia. bits in 11 years doing it this way!
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 3162
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Compression bit and cutting strategy in Cut2D

Postby potzmannwoodshop » Fri Jun 29, 2018 2:03 pm

mtylerfl wrote:Yes, that is what I was referring to also. You gotta get that bit to proper depth before it starts cutting the “good part” of the material so the upcut portion of the bit isn’t “ripping up” the top of it.

For 0.5” thick material, it shouldn’t be a problem cutting full-depth anyway. I cut up to 0.75”-thick Pine and Poplar at full-depth on the CarveWright CNC when using a 0.125” dia. EM. Hardwoods do require shallower pass depths...I’ll set pass depths at 0.3” or 0.4” on the CarveWright. I’ve broken only two 0.125” dia. bits in 11 years doing it this way!



Speeds and feeds for a .125" cutting full depth .5"? Im just curious, I usually cut .5" with a .25" compression at 250ipm and .75" with a .5" compression at 350ipm.
potzmannwoodshop
Vectric Apprentice
 
Posts: 79
Joined: Wed Feb 15, 2017 2:03 pm
Model of CNC Machine: 2 SCM Routech Record 120s(1999, 2001)

Re: Compression bit and cutting strategy in Cut2D

Postby mtylerfl » Fri Jun 29, 2018 2:31 pm

The CW CNC feeds/speeds are pre-set from the factory.

The 0.125” dia. EM is a 4-flute upcut. The max rpm for the CW is 20k, but I’m guessing the rpm are about 18k when performing a cut operation.

The bit enters the cut with a ramp of about 1” and I estimate it’s set at about 0.3 ips. After full depth is reached, it appears to move at 0.4 to 0.5 ips
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 3162
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha


Return to Cut2D - General

Who is online

Users browsing this forum: No registered users and 8 guests