PDA

View Full Version : What bits to use? what speed etc?



dray
03-11-2007, 11:21 PM
I bought the basic setup package of onsrud bits from Shopbot with my prs alpha.

I was curious how fast and how deep most of you cut mdf, ul mdf, baltic birch which bit is best for production cabinetry etc..

Any help at all is appreciated greatly.

Thx

jwool
03-12-2007, 04:15 AM
Danny, im running Alpha120/Columbo spindle, i recently have been asking similar questions, b/c of breaking bits ( 1/4 inch endmill 2flute upcut, SB tells me to use the Chip Load calculator, but then they say its not an exact science, rather its a trial and error process. I use Onsrud bits, but am thinking about switching to Whiteside bits because of the praise Frank gives them.

I cut 3/4 MDF single pass around 17,000 rpms which is .007 chip load. The bits i use call between .006 to .008 . I called Onsrud and talked to their tech guys, helped out alot, i'm starting to think that my parts might be moving while being cut ( due to a rough looking spoil board that needs resurfacing ).

Im still a newbie, but i have asked the same question before and frequently.. Not sure if i helped you, but i looked @ the new videos on SB's site & they are cutting 3/4 mdf @ 6IPS single pass.

Once i figure out my problem, i'll be more than glad to pass along the info to you

hines
03-12-2007, 09:54 AM
I am using a 2 flute 1/4 inch solid carbide spiral downcut from CMT (first nice bit I bought, no other reason). Just the other day I ran a test on feed and rpm speeds with my PC router and I cut 10 36 inch lines with 1 pass into a sheet of 3/4 MDF. I increased the feed by .5 ips on every line and 3,000rpm on every 2 lines (keeping up with chip load calculations of .010 to .020). I went from 3 ips at 10k rpm all the way to 7.5 ips at 21k rpm. The sweet spot was about 6 ips at 19k. Any faster than that and the bit got higher pitched, I felt like it was gonna break off. Hope this helps, it gave me a lot of info on the bots capabilities.

richards
03-12-2007, 10:03 AM
The chipload calculator works great for the kind of work that I do (mostly long straight cuts in cabinet parts). However, I start at 0.015 chipload and go larger to 0.020 or 0.025 whenever possible. My spindle can handle that size of cut without bogging down. Normally, I'm comfortable running MDF, particle board and melamine at 7-10 ips. Sometimes I go slower if things don't sound quite right (different batches probably had different amounts of glue or other manufactured differences that warrant minor changes in feed speed). When I have a choice, I'd rather use a 1-flute spiral down cutter. My vacuum isn't strong enough to allow through cuts, so I don't use compression cutters.

An easy way to make tests is to make a series of straight cuts at least 24-inches long at different feed speeds (5, 6, 7, 8, 9, 10 ips). Compare the cuts. The first one that shows too much roughness is the speed that is too fast for that cutter at that RPM. What I like to get are hot chips and good edge quality. That means that the chip is pulling the heat away from the cutter and that the quality isn't suffering.

bjs
03-13-2007, 07:43 PM
Mike, you said your vacuum isn't strong enough, just curious what vac system your running. I am looking at buying a router for cutting cabinet parts. Am wondering what I need for 1 pass through cut on 3/4" melamine.

richards
03-13-2007, 08:55 PM
Brent,
I have two Fein vacuums; however, I'm at 4,500 feet altitude, which really reduces the atmospheric pressure. Other users who are nearer sea-level seem to have much greater hold-down pressure than I do.

Also, I have no trouble at all holding down any cabinet sized part when I use a GAST pump with a vacuum mask, but that means that I would have to create a vacuum mask for each variation of each 4x8 sheet of material. The GAST generates over 21" of mercury - but allows absolutely no leakage. The Fein vacuum generates 5" of mercury - but allows the use of a standard vacuum plenum and bleeder board.