How deep are you cutting?
With a depth of cut of about .01", I'd think maybe 300-400ipm at 17,000 rpm.
But, I've never used one of those.
This isn't a CNCRP specific question, but since I have a CRP4896, thought I'd give it a try.
Having problems getting a feed/speed for the RC-2251 bit that won't burn the MDF. Toolstoday video on surfacing using this tool recommends 100 ipm @ 12000 rpm, but I only got a few feet before the burning started. Amana's data says 17000 rpm @ 60 ipm , but that seems way too slow. I must be missing something. Anyone out there have this bit that can help me out? Thanks.
Similar Threads:
How deep are you cutting?
With a depth of cut of about .01", I'd think maybe 300-400ipm at 17,000 rpm.
But, I've never used one of those.
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Are chips packing into the bottom cutters?
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
I have been using this cutter: https://www.amazon.com/gp/product/B0...?ie=UTF8&psc=1
At 18000RPM and 500IPM .050in DOC 1.75in WOC
Surfaces the entire 49x97inch table in about 8 minutes.
This video from toolstoday shows them moving much faster.
Any chance your inserts are not sharp? That can cause burning.
Otherwise, travel faster.
Cheers
Roger
I just did mine a few weeks ago. I went shallower - 0.010 or so and around 120 ips. No issues. I ended up taking a couple of passes to get a complete "fresh" surface. Not sure what the RPM was - Bosch 1617 turned down a notch from full speed - still sounded like a helicopter!
Tony
The bit and inserts are new (just got it yesterday). BUT, maybe I dulled them out by using the speeds/feeds shown on the toolstoday video! I didn't rotate them before I tried faster speeds and feeds. Didn't occur to me that they would have dulled out that fast, but maybe so.
Made several more attempts and finally got a decent result using settings close to the Toolstoday video. 110 ipm , 12K rpm, .030 doc. Took a long time, but I was getting a small chip rather than dust. Increasing the feedrate seemed to make the most difference. Now, I'll see how it does on slabs. Thanks for the input guys!
Sorry, no I have the less expensive two cutter model. Glad you got some better results.
Thanks Tony. Apparently, Toolstoday (and Amana I guess) considers the 2251 a 2 flute cutter also ("2+2"), as in 2 cutters + 2 scorers. That's the only way I can make sense of Amana's feed/speed chart and how Toolstoday came up with their feed/speed. If you calculate as a 2 flute with 12000 rpm it calculates to 96 ipm, though like I said, a bit higher feed worked better for me. I may try kicking up the numbers next time, but for now I just wanted it done!
I was getting burning as well. I never got it just right just accepted it
I used the same bit to surface my spoilboard. I found that the bottom cutting bits are slightly recessed from the side bits. If you take a shallow cut, the bottom bits just sit there and burn.
I found two solutions. First is to remove the bottom bits and make shallow cuts with just the side bits. Keep increasing the feedrate. I pushed mine close to 200 IPM at 18000. Second is to keep the bottom bits on, but make a deeper cut.
that will engage the bottom bits so that they actually cut and not burn. I was able to surface the 4x8 sheet with one pass using only the side bits and not stopping in the middle to rotate them.
the bottom cutting bits are slightly recessed from the side bits.
I have never used one of these, so treat my comments accordingly.
But that sounds very strange. I would have expected the bottom bits to stick down below the side bits.
Are the mounting faces clean and the inserts properly mounted?
Have you contacted Amana to ask about this?
Merry Xmas
Roger
No I never contacted them. I just use it with the two side bits and call it a day!!!
Anyone figure this bit out yet?
As I posted above, I was able to get decent results (with all 4 bits installed) using Toolstoday's recommended settings per their video with a 10-15% higher feedrate. However, looking back I really think all my troubles begin with one major rookie mistake. I knew I couldn't plunge with this bit so (logically I thought), I decided to do a long ramp in (about 12" as I recall). Problem was I didn't change the plunge rate (which was at Vectric's default of 30 ipm). I guess because I had brand new bits (?) it managed to not burn with the first ramp/plunge so I didn't make the connection. Looking back at the TT video, I saw that they started off to the side of spoilboard which would be the way to go if you have the open space to do so. Sooooo, after finally realizing my mistake and ramping or starting at depth in open space at 110 ipm, I've had no problem. Learning the hard way can be expensive. Hope this might be of help.