Help Please

This forum is for general discussion regarding VCarve Pro

Help Please

Postby neshra » Fri Jun 01, 2018 8:36 pm

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?
Attachments
pocket.jpg
neshra
 
Posts: 21
Joined: Wed Feb 01, 2017 9:41 am
Location: Laguna Niguel CA
Model of CNC Machine: ShopSabre 23

Re: Help Please

Postby ChrisInEstes » Fri Jun 01, 2018 8:44 pm

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
Aspire 8.5 - PhotoVCarve - FlexiEXPERT 11
User avatar
ChrisInEstes
Vectric Wizard
 
Posts: 798
Joined: Fri Jul 17, 2009 8:00 pm
Location: Estes Park, Colorado, USA
Model of CNC Machine: Vytek 4' X 8' - Perske Spindle - Mach3

Re: Help Please

Postby Ken Tipton » Fri Jun 01, 2018 8:45 pm

I would try using a down cut bit.
Ken Tipton
 
Posts: 42
Joined: Mon Feb 06, 2017 7:07 pm
Location: Ladera Ranch CA
Model of CNC Machine: Laguna IQ

Re: Help Please

Postby neshra » Fri Jun 01, 2018 8:56 pm

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
Attachments
IMG_5108.jpg
IMG_5107.jpg
IMG_5109.jpg
neshra
 
Posts: 21
Joined: Wed Feb 01, 2017 9:41 am
Location: Laguna Niguel CA
Model of CNC Machine: ShopSabre 23

Re: Help Please

Postby ChrisInEstes » Fri Jun 01, 2018 9:00 pm

That looks like what I get when I use upcuts.... My downcuts are near perfect, and require almost no cleanup.
Aspire 8.5 - PhotoVCarve - FlexiEXPERT 11
User avatar
ChrisInEstes
Vectric Wizard
 
Posts: 798
Joined: Fri Jul 17, 2009 8:00 pm
Location: Estes Park, Colorado, USA
Model of CNC Machine: Vytek 4' X 8' - Perske Spindle - Mach3

Re: Help Please

Postby Rcnewcomb » Fri Jun 01, 2018 11:02 pm

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
User avatar
Rcnewcomb
Vectric Wizard
 
Posts: 3076
Joined: Fri Nov 04, 2005 5:54 am
Location: San Jose, California, USA
Model of CNC Machine: GCnC/WinCNC

Re: Help Please

Postby neshra » Sat Jun 02, 2018 12:33 am

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:
neshra
 
Posts: 21
Joined: Wed Feb 01, 2017 9:41 am
Location: Laguna Niguel CA
Model of CNC Machine: ShopSabre 23

Re: Help Please

Postby Daniel S » Sat Jun 02, 2018 3:10 am

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 .
Daniel S
Vectric Apprentice
 
Posts: 50
Joined: Thu Jan 08, 2009 6:24 am
Location: Orange, CA
Model of CNC Machine: Shark HD4

Re: Help Please

Postby mark-s » Sat Jun 02, 2018 3:26 am

Down cut bit will fix that.
mark-s
mark-s
Vectric Apprentice
 
Posts: 61
Joined: Sat Feb 03, 2018 2:03 am
Model of CNC Machine: diy cnc router

Re: Help Please

Postby SCW » Sat Jun 02, 2018 5:08 am

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.
SCW
 
Posts: 26
Joined: Fri May 11, 2018 4:44 am
Location: Stillwater, MN
Model of CNC Machine: Axoim AR8 Pro+ (w/ 4th axis); Aspire 9.0

Re: Help Please

Postby neshra » Sat Jun 02, 2018 6:08 am

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.
neshra
 
Posts: 21
Joined: Wed Feb 01, 2017 9:41 am
Location: Laguna Niguel CA
Model of CNC Machine: ShopSabre 23

Re: Help Please

Postby scottp55 » Sat Jun 02, 2018 2:01 pm

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-CARBIDE-2-FLUTE-ENDMILLS-DOWN-CUT-FOR-SOFT-PLASTIC-1650-1250-500/381784780650?hash=item58e4256f6a:g:-mQAAOxyH89Q2Lce:sc:USPSFirstClass!04429!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 :D
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.
User avatar
scottp55
Vectric Wizard
 
Posts: 2302
Joined: Thu May 09, 2013 11:30 am
Location: Kennebunkport, Maine, US
Model of CNC Machine: Shopbot Desktop 5.5"Z/spindle/VCP9

Re: Help Please

Postby mark-s » Sat Jun 02, 2018 2:18 pm

There is 1/8 inch downcut bit available, also 1/16 inch downcut.
I have used both with maple and oak.
mark-s
mark-s
Vectric Apprentice
 
Posts: 61
Joined: Sat Feb 03, 2018 2:03 am
Model of CNC Machine: diy cnc router

Re: Help Please

Postby neshra » Sat Jun 02, 2018 10:15 pm

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
Attachments
IMG_5433 (1).jpg
IMG_5432.jpg
neshra
 
Posts: 21
Joined: Wed Feb 01, 2017 9:41 am
Location: Laguna Niguel CA
Model of CNC Machine: ShopSabre 23

Re: Help Please

Postby tomgardiner » Sun Jun 03, 2018 9:36 pm

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.
tomgardiner
Vectric Craftsman
 
Posts: 286
Joined: Thu Oct 02, 2014 1:49 pm
Model of CNC Machine: FMT Patriot 4 x8

Next

Return to VCarve - General

Who is online

Users browsing this forum: dwilli9013, steve323 and 23 guests