Help Please
-
- Posts: 23
- Joined: Wed Feb 01, 2017 9:41 am
- Model of CNC Machine: ShopSabre 23
- Location: Laguna Niguel CA
Help Please
Hello All,
I am pocketing these Hard Maple pieces on my CNC and using 5 parts at each giving time. the pocketing size is 1.8"Lx0.5"Wx0.5"D. In every batch I get one that comes out with one side splintering like the photo.
I am using Whiteside 1/8" Spiral up Cut, 2 Flute. My setting in VCarve are: "Offset" Clear Pocket, using climb. Tool: 16000 rpm, 100 - 160 I/M feed rate (I tried 100, 140, 145, and 160), and 30 I/M plunge rate, ramping 0.3".
I have not tried Raster since it is taking longer nor have I tried Conventional instead Climb.
I am not sure if it is the wood or the bit or my setting??
Any suggestions?
I am pocketing these Hard Maple pieces on my CNC and using 5 parts at each giving time. the pocketing size is 1.8"Lx0.5"Wx0.5"D. In every batch I get one that comes out with one side splintering like the photo.
I am using Whiteside 1/8" Spiral up Cut, 2 Flute. My setting in VCarve are: "Offset" Clear Pocket, using climb. Tool: 16000 rpm, 100 - 160 I/M feed rate (I tried 100, 140, 145, and 160), and 30 I/M plunge rate, ramping 0.3".
I have not tried Raster since it is taking longer nor have I tried Conventional instead Climb.
I am not sure if it is the wood or the bit or my setting??
Any suggestions?
- ChrisInEstes
- Vectric Wizard
- Posts: 841
- Joined: Fri Jul 17, 2009 8:00 pm
- Model of CNC Machine: Vytek 4' X 8' - Perske Spindle - Mach3
- Location: Estes Park, Colorado, USA
Re: Help Please
I'd use a downcut spiral bit. I get mine from 2L, Inc. I route lots of hard maple, and have great results with downcut spirals.
Chris
Chris
Aspire 9.5 - FlexiEXPERT 11 - Vytek Rebel 4' x 8' - 5HP Perske Spindle
-
- Vectric Apprentice
- Posts: 70
- Joined: Mon Feb 06, 2017 7:07 pm
- Model of CNC Machine: Laguna IQ
- Location: Ladera Ranch CA
Re: Help Please
I would try using a down cut bit.
-
- Posts: 23
- Joined: Wed Feb 01, 2017 9:41 am
- Model of CNC Machine: ShopSabre 23
- Location: Laguna Niguel CA
Re: Help Please
I have used down cut before and I get lots fuzz and have to spend time to clean them up. I am attaching photos from those with down cut
- ChrisInEstes
- Vectric Wizard
- Posts: 841
- Joined: Fri Jul 17, 2009 8:00 pm
- Model of CNC Machine: Vytek 4' X 8' - Perske Spindle - Mach3
- Location: Estes Park, Colorado, USA
Re: Help Please
That looks like what I get when I use upcuts.... My downcuts are near perfect, and require almost no cleanup.
Aspire 9.5 - FlexiEXPERT 11 - Vytek Rebel 4' x 8' - 5HP Perske Spindle
- Rcnewcomb
- Vectric Archimage
- Posts: 5887
- Joined: Fri Nov 04, 2005 5:54 am
- Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
- Location: San Jose, California, USA
- Contact:
Re: Help Please
You might try a different brand of bit. I like Whiteside, but sometimes another brand has a slightly different geometry that works better for certain materials. Take a look at Centurion Tools.
- Randall Newcomb
10 fingers in, 10 fingers out, another good day in the shop
10 fingers in, 10 fingers out, another good day in the shop
-
- Posts: 23
- Joined: Wed Feb 01, 2017 9:41 am
- Model of CNC Machine: ShopSabre 23
- Location: Laguna Niguel CA
Re: Help Please
The places that I know around me is Woodcraft that I think carries only FREUD and WhiteSide and Austin Hardwood that carries Amana Tools.
This is in Amana's description for Straight Cut 2 Flute 1/8":
Use a two-flute bit where fine finish is paramount. Two flutes balance the bit, eliminating vibration that degrades the cut finish. Two cuts per revolution yield a smooth surface, but feed rate is slightly reduced. 45200 features a solid carbide cutting edge.
Excellent for Cutting:
This is in Amana's description for Straight Cut 2 Flute 1/8":
Use a two-flute bit where fine finish is paramount. Two flutes balance the bit, eliminating vibration that degrades the cut finish. Two cuts per revolution yield a smooth surface, but feed rate is slightly reduced. 45200 features a solid carbide cutting edge.
Excellent for Cutting:
-
- Vectric Craftsman
- Posts: 110
- Joined: Thu Jan 08, 2009 6:24 am
- Model of CNC Machine: CAMaster Stinger SR-23
- Location: Orange, CA
Re: Help Please
I had a very similar problem when trying to cut pockets in alder & hard maple when making business card holders. I purchased a 3/16 3-flute fish-tail end mill from Precise Bits and it solved all my problems. I requires the purchase of collet to match 3/16 dia of end mill. I use it when cutting out and when pocketing holes. My machine is not the ridged machine I had hoped for but slowing down feed rate worked for me, even through the bit is designed for hi feed rate and deep cuts. Just sharing my experience with this bit .
-
- Vectric Craftsman
- Posts: 216
- Joined: Sat Feb 03, 2018 2:03 am
- Model of CNC Machine: diy 4 X 4 CNC Router
- Location: So. Cal.
Re: Help Please
Down cut bit will fix that.
mark-s
mark-s
-
- Posts: 26
- Joined: Fri May 11, 2018 4:44 am
- Model of CNC Machine: Axoim AR8 Pro+ (w/ 4th axis); Aspire 9.0
- Location: Stillwater, MN
- Contact:
Re: Help Please
It would be interesting to know your speed, feed, and pass depth. It kind of looks from the picture that you might be plunging and routing fairly deep on any given pass.
I've bought the cheap 6-pc, 2-flute, up-cut ball nose and end mill kits off of Amazon and had great results. I'm typically running them at 15,000-18,000 rpm; I typically set up my end mill tool path for 1in/sec or less; I plunge up to 1/2 of the diameter but usually no more than 1/8" per pass. And I usually set my handheld controller to run the program at 50-75% of commanded speed. I've found that these settings prevent all chip out and burning from my carvings.
I've bought the cheap 6-pc, 2-flute, up-cut ball nose and end mill kits off of Amazon and had great results. I'm typically running them at 15,000-18,000 rpm; I typically set up my end mill tool path for 1in/sec or less; I plunge up to 1/2 of the diameter but usually no more than 1/8" per pass. And I usually set my handheld controller to run the program at 50-75% of commanded speed. I've found that these settings prevent all chip out and burning from my carvings.
-
- Posts: 23
- Joined: Wed Feb 01, 2017 9:41 am
- Model of CNC Machine: ShopSabre 23
- Location: Laguna Niguel CA
Re: Help Please
my r.p.m. is 16000, my feed rate i tried between 100 to 160 I/M and my plunge rate is 30 I/M and on each pass I am taking 1/8" material.
I will try 2 things tomorrow:
1. Slower speed (however I have to finish about 800 of them this weekend and laser engrave a logo on the top of them)
2. Use a down cut bit.
The client likes the small corners of 1/8 bit and I am not sure if he will like the larger corners if I use 3/16 bit. He did not like the 1/4 at all.
I will try 2 things tomorrow:
1. Slower speed (however I have to finish about 800 of them this weekend and laser engrave a logo on the top of them)
2. Use a down cut bit.
The client likes the small corners of 1/8 bit and I am not sure if he will like the larger corners if I use 3/16 bit. He did not like the 1/4 at all.
- scottp55
- Vectric Wizard
- Posts: 4713
- Joined: Thu May 09, 2013 11:30 am
- Model of CNC Machine: ShopbotDesktop 5.5"Z/spindle/VCP11.5
- Location: Kennebunkport, Maine, US
Re: Help Please
Just 2 cents, but in most hardwoods with a downcut bit I get much better results with a conventional toolpath.
For that toolpath I'd definitely do a downcut, and if it's a .125" bit, then Drillman1's .125" down is VERY hard to beat for good pockets with little to no sanding.
https://www.ebay.com/itm/1-8-1250-CARBI ... 4429!US!-1
Fast reliable service on all my many orders. And pretty painless to swap out when dull, but they last VERY well.
I like ALL his 1/8" bits except his 30 degree "Sharp". It says soft plastic, but then Teak/Bloodwood/and other dense hardwoods are soft plastic
For Sugar Maple, it likes .8-1IPS at 1/2 bit diameter and 16-17K for the best cut...adding a last pass depth of .015" will pretty much eliminate sanding pocket bottoms. I'm finicky as heck though, and mostly one ofs nowadays...for production I'd probably wind up around 1.5IPS/deeper passes/after slowly increasing speeds/feeds/pass depth.
scott
For .25" downcuts I like the Centurion FEM Downcut for pockets.
For that toolpath I'd definitely do a downcut, and if it's a .125" bit, then Drillman1's .125" down is VERY hard to beat for good pockets with little to no sanding.
https://www.ebay.com/itm/1-8-1250-CARBI ... 4429!US!-1
Fast reliable service on all my many orders. And pretty painless to swap out when dull, but they last VERY well.
I like ALL his 1/8" bits except his 30 degree "Sharp". It says soft plastic, but then Teak/Bloodwood/and other dense hardwoods are soft plastic
For Sugar Maple, it likes .8-1IPS at 1/2 bit diameter and 16-17K for the best cut...adding a last pass depth of .015" will pretty much eliminate sanding pocket bottoms. I'm finicky as heck though, and mostly one ofs nowadays...for production I'd probably wind up around 1.5IPS/deeper passes/after slowly increasing speeds/feeds/pass depth.
scott
For .25" downcuts I like the Centurion FEM Downcut for pockets.
Last edited by scottp55 on Sat Jun 02, 2018 2:30 pm, edited 1 time in total.
I've learned my lesson well. You can't please everyone,so you have to please yourself
R.N.
R.N.
-
- Vectric Craftsman
- Posts: 216
- Joined: Sat Feb 03, 2018 2:03 am
- Model of CNC Machine: diy 4 X 4 CNC Router
- Location: So. Cal.
Re: Help Please
There is 1/8 inch downcut bit available, also 1/16 inch downcut.
I have used both with maple and oak.
mark-s
I have used both with maple and oak.
mark-s
-
- Posts: 23
- Joined: Wed Feb 01, 2017 9:41 am
- Model of CNC Machine: ShopSabre 23
- Location: Laguna Niguel CA
Re: Help Please
I started today with 1/8" downcut from Onsrud and shimming the sides to make sure not even 0.01" gap and it seems to be working much better
-
- Vectric Wizard
- Posts: 447
- Joined: Thu Oct 02, 2014 1:49 pm
- Model of CNC Machine: FMT Patriot 4 x8
Re: Help Please
Vibration from loose fit in your jig is going to be a major contributor to chatter and poor finish.
If this is a regular gig I suggest you tweak the holding jig some. I hold workpieces in a similar fashion often in a small production basis. I made cnc cut wedges that work on all my jigs. When I make jigs I incorporate the mating taper for the wedges. The key I found is to reduce the load and unload time. I cut the wedges with a nominal 5/16" hole and made a lock and remove tool with a steel dowel to tap the wedges tight and loose. Shims are slow to jamb in place and sometimes you don't have what you need when you need it.
Sorry, I am not at the computer to give an illustration.
If this is a regular gig I suggest you tweak the holding jig some. I hold workpieces in a similar fashion often in a small production basis. I made cnc cut wedges that work on all my jigs. When I make jigs I incorporate the mating taper for the wedges. The key I found is to reduce the load and unload time. I cut the wedges with a nominal 5/16" hole and made a lock and remove tool with a steel dowel to tap the wedges tight and loose. Shims are slow to jamb in place and sometimes you don't have what you need when you need it.
Sorry, I am not at the computer to give an illustration.