MechMate CNC Router Forum

MechMate CNC Router Forum (http://www.mechmate.com/forums/index.php)
-   Cutting various materials - bit selection, feeds, speeds (http://www.mechmate.com/forums/forumdisplay.php?f=82)
-   -   Speeds, Feeds, Materials and Bits (http://www.mechmate.com/forums/showthread.php?t=724)

smreish Wed 05 March 2008 11:59

News Flash.
New product I have NEVER cut on the table before just arrived. I ordered 20 sheets...we will see how it does.
I even ordered fancy schmancy bits to cut all of it.
The product.
3/4" cabinet grade birch
laminated 1 or 2 sides with various types of High pressure plastic laminate. This way, my cabinets are prefinished on all of the interior surfaces. Tonight should be fun :D

Gerald D Wed 05 March 2008 12:12

"Compression" schmancy bits?

smreish Wed 05 March 2008 12:41

You betcha! Compression spiral 1/4" 7/8 CL, 2.25 OAL
I also order solid carbide, straight cut, 2 flute *onsrud* plastic cutting bits as well. Just in case.
It's all about the testing :)

smreish Fri 07 March 2008 01:48

Gerald.
Those fancy schmancy compression bits and 20 sheets of laminated core plywood are NO match for the MechMate. I flew through 20 sheets in 4 hours this morning.
Stats:
1/4" compression spiral and 1/4" carbide, 2 flute straight cut bits.
- both performed equally well.
- better cut edge with 2 flute
- better chips with compression.
- avg speed 180ipm with 2 passes .30 inch/pass

I will be cutting 3/8" polycarbonate, 1/4" acrylic tomorrow ( well, in about 5 hours :)

Gerald D Fri 07 March 2008 02:22

Surely the compression cutter only works for one full depth pass? From what I read of the regular compression cutter users, they rarely cut material thicknesses more than 2X cutter diameters thick. ie. a 3/8" cutter for 3/4" material.

Marc Shlaes Sun 27 April 2008 16:50

Speeds, Feeds, Materials and Bits
 
JR and I have been cutting a whole lot of interesting "one-offs" while learning to use the beast. We have cut MDF, Baltic Birch plywood, PVC, Expanded PVC, ABS, Alumin(i)um, etc. Each time we have to learn the hard way about proper speeds and feeds for the bit and the material. It seems that this thread could be a way for us (and others) to share that experience so that absolutely everything does not have to be learned the hard way by absolutely everyone.

When you think about the combination of bit (up-cut / down-cut, compression cut, straight cut), material, cut depth, plunge rate, ramp angle, ramp speed, cut speed, step-over (on a pocket cut), rough cut, climb cut, finish pass, spindle speed, etc... it can get overwhelming.

But, an understanding of all those things (and more) is what it takes.

Let's capture and share our experiences. The group can decide what is good and bad. I look forward to it.

Thanks.

smreish Sun 27 April 2008 20:19

....Ohhh Marc, that is what makes Big Blue perform it's best. Knowing the secret of cutting tool vs. material vs. speed.
I'm in.

Okay, based on my most recent post using 3/8" acrylic.
Spiral Up, Onsrud 1/4" plastic bit. #52-624
19,000 Rpm
climb cut
125 ipm.
Never exceeded .2875 per pass.
Pocketing, boring and final cut out.
NO tabbing.

Marc Shlaes Sun 27 April 2008 20:40

Sean, thanks for jumping in!

We have been using general purpose carbide router bits primarily from Freud. We haven't invested in "CNC" bits nor those specifically designed for a material such as acrylic or aluminum. Should we be doing more looking at "more higher end" bits?

We have seen TREMENDOUS (really unbelievable) wear on bits in MDF. The best performance that we seem to get is when we employ shallow, rather slow ramping, and then go as fast as you can. It seems that heat is causing real problems if you go too slowly.

With JR's non-geared motors, we have run into significant issues especially plunging. We have designed and fabricated prototypes of belt drives to try to alleviate those issues so our plunging speed and ramp angles have been purposely slow and shallow. We will see if we can / should speed up the cut entry after the belt drives are deployed.

We also learned that you simply can't plunge a downcut spiral straight into MDF (as a drill process) at really any speed. We actually caught MDF on fire. The excitement didn't make it to the dust collector though. That could have been really exciting. :eek:

I am compiling a spreadsheet of our thoughts and experiences and then we will post that as a starting point.

Sean, what are you doing instead of tabbing? Specialized holddowns? Vacuum?

smreish Sun 27 April 2008 21:58

Marc,
Good bits do wonders for the MDF cutting.
When the chip clears, very little is left to burn :)
Hold downs are currently via the Gerald G clamp method and multiple passes.
I usually leave about a .030 skin on the bottom of the part to keep in place then sand the "chip" off once I pull the part.
Otherwise, just leave the last pass to a tiny thickness and the part doesn't really move on me.
I tab occasionally, but only on 1/8 and 1/4 plastic sintra or polycarbonate. And for those I usually put down a few strips of doublesided carpet tape. Viola! Hold down.
If you really need to drill, then I recommend actually making 2 cut files and run the drill sequence with a real drill bit, then run the second file to cut the part. A little extra time, but without a tool changer, its your best tool life saving option.
The "real" bits only cost about 20 dollars - about the same as a frued at the home centers - but make a world of difference. I also found that real MEtal endmill bits from MSC catalog cut MDF REALLY well.

Vacuum coming when I move the machine to it's new home.

Gerald D Sun 27 April 2008 23:43

Quote:
Originally Posted by smreish View Post
I also found that real MEtal endmill bits . . . . . . cut MDF REALLY well.
Fully agree!

Also, for MDF, there is no such thing as "standard" MDF. Over here we have a choice of two types:
- Truepan, an import, has a more yellowish colour, is consistent in density from outside to center. Cuts easy, tools last long.
- Generic locally produced MDF, more red/brown colour, hard outer skins with softer center. Find a glue build-up on the cutter and give a much shorter cutter life.

Gerald D Sun 27 April 2008 23:49

Key to this discussion is "chipload"; which is the thickness of the shaving that each blade of the cutter removes as the tool advances. Influenced by:
1 Move speed
2 Rotation speed
3 Number of tips on the cutter

Much has been said all over the internet, and by tool suppliers on chipload.

isladelobos Mon 28 April 2008 05:48

This is the density, type, size and weight of DMF in spain.

http://www.bricotodo.com/tipostableros.htm

cncb Thu 29 May 2008 04:25

Looking good Sean. How many sheets do you go through each day? 30 router bits sounds a bit much for one month, even with MDF. How many times do you change the dust collector bags for the router every week? :D

smreish Thu 29 May 2008 06:33

Brian,
Depends on poorly I treat the bits!:eek:
Some days, I get 10 sheets on a bit, sometimes only 1!
My challenge is I rarely cut MDF...usually some weird lay-up of plastic on wood. Aluminum with Plastic. Plastic only. PVC/ Sintra. OSB for template stuff. Real Oak or Maple. Cardboard - yep cardboard. Just to name a few things I have been cutting.

cncb Fri 30 May 2008 04:44

:D go try and cut Jatoba or Ebony, there are some exotic south american woods that cut like steel or sheet metal its nuts. But with good solid carbide tooling you shouldn't be going through that many router bits. You ever look into a higher quality spiral where you can buy a few sets and send them out to be sharpened?

smreish Fri 30 May 2008 07:04

All the bits I have are high quality onsrud carbide. I just can plan for the occasional "operator" usage. Hit a clamp while jogging, etc. Plunge to fast and burn the bottom....using the wrong bit on the wrong material. Like wood carbide bit on aluminum sheet. All things I am certain the guys in the shop will learn and my use will go down.

....learning curve a little higher than normal for some of my shop guys!

Alan_c Fri 30 May 2008 09:30

Try pushing them faster, I found with MDF that they burn easily from rubbing if the feed speed is too slow. My good mate George Hess (ex MultiCam agent) used to tell me push them as fast as possible until just before they break then back off slightly...:)

smreish Fri 30 May 2008 10:07

Alan,
Good advice. I'll try that...in about 6 minutes when the next cut is done!
Back to making wood chips and lots of dust.

Robert M Fri 30 May 2008 10:22

Sean
May not be any news but worth reminding, make your self a favor, download Onsrud main 2006 cutter catalog & have a look at the technical data at the end, from p78 on. Chip load & tool staying at proper temp is the approach, not till they break :confused:

Amiclalement, Robert ;)

IN-WondeR Fri 30 May 2008 17:04

Speeds, Feeds, Materials and Bits
 
Where do you guys buy your Router bits...
I'm looking around for some good quality Solid Carbide bits....

smreish Fri 30 May 2008 18:14

To address all out there on bits. I have the Onsrud chart comfortably placed on the wall and refer to it ever time the table fires up. After all the years running the Multicam, Bridgeport and others, you get accustomed to the "feel and sound" of each tool bit.

I found out later today that the 13 dollar 3/8" shank, 2 flute tin coated 1/4" diamter cutting bit from McMaster Carr (a metal cutting bit) did a fantastic job on the MDF. It always does. I also ran it without issue at 225ipm per 3/8 " pass. Great chip load...no smoke...still sharp.

I certainly don't want to change my personal thread to a bit / tool discussion. I just thought the new members and novice folks would appreciate a little insight when I try something a little new.

Happy cutting ya'll.

Sean

smreish Fri 30 May 2008 18:16

Oh gosh.
I get deals everywhere.
Piedmont plastics sells onsrud
Hartlauer Bits sells bosch, onsrud and others.
McMaster carr Sells what ever they get the best deal on.

I use them all.

Even Frued from HomeDepot, but they don't usually hold up well because they are often carbide tipped and not solid carbide.

Greg J Mon 09 June 2008 18:49

Quote:
Originally Posted by smreish View Post
I found out later today that the 13 dollar 3/8" shank, 2 flute tin coated 1/4" diamter cutting bit from McMaster Carr (a metal cutting bit) did a fantastic job on the MDF. It always does. I also ran it without issue at 225ipm per 3/8 " pass. Great chip load...no smoke...still sharp.
Sean,

Could I get that McMaster P/N from you. I'm new at this and there are so many different bits to choose from.

smreish Mon 09 June 2008 20:51

some quick bit choices I use from McMaster Carr
 
27395A25
Carbide Router Bit for Wood and Laminates Up-Cut, 1/4" Cut Dia, 1" Cut Length, 2-1/2" L O'all
Spiral UP!
In stock at $20.70 Each
SUPERB cut in PVC, SINTRA, WOOD laminate layup and most plastics.

8876A63
General Purpose Two-Flute Carbide End Mill 1/4" Mill Dia, 1/4" Shank Dia, 3" O'all Length
In stock at $17.04 Each
Just fine for all your MDF and PLY needs. NIce smooth cut. Last's pretty well for a solid carbide bit.

8876A17
General Purpose Two-Flute Carbide End Mill 1/4" Mill Dia, 1/4" Shank Dia, 2-1/2" O'all Length
In stock at $13.65 Each *this is a great - cheap solution but requires you to make at LEAST 2 passes on cutting 3/4"
material to utilize the 3/4" cutting surface allowance. I currently set up Mach to cut .385/pass @ 230 ipm and works well in
MDF and PLYwood.

Since I cut A LOT of 1/2 AND 1/4" MATERIAL this is a nice - cheap choice for the shop.

Good luck ya'll

Marc Shlaes Mon 09 June 2008 21:06

Sean (or anyone else)

Got to do some thru cutting in 1.5" oak. Would like to use a 1/4 inch bit to minimize kerf. Got any opinions regarding bits / speeds / feeds???

Thanks.

smreish Mon 09 June 2008 21:21

Marc,
Oak...has it's challenges.
The success I had recently is think of it like aluminum....that shatters.
The long open grain in oak really requires you to take A LOT of passes.
MY memory serves me correct.
for 5/4 material I made 5 passes @ 90 IPM.
The end result was a curved handrailing that was pocket holed back together on the quadrants of the circle.

I used a solid carbide, solid flute 1/4" bit.

Good luck.
Sean

Greg J Mon 09 June 2008 21:46

Thanks Sean,

Your's and Marc's post help allot.

Placing order for bits right now. :)

Greg J Sun 07 December 2008 11:01

Pass Depth
 
Is there a general rule on pass depth? I have not seen any discussion and the feed rate calculation does not have pass depth in the formula.

Some have suggested running feed rates fast until breakage. Breaking HSS rotating at 10K to 20K does not sound like the kind of experimenting I want to do.

I have not broken any bits ... yet ... my general rule is currently 50% of diameter for pass depth. Can I go 100%, 110%, etc of diameter.

I know the material being cut is everything, so for discussion purposes, lets stay with hard woods. Oak, Walnut, Ash, etc. Lets also not worry about finish of cut (that's easy to experiment with safely). What pass depth for a thru cut?

What happens when a bit snaps due to high loading?

Gerald D Sun 07 December 2008 11:11

We sort of go 2X diameter on soft wood and 1X diameter on hardwood.

To reduce chances of bits snapping, keep them as short as possible, as deep in the collet as possible.

Bits snapping are very rare. Have not had a serious missile yet. The centrifugal force on a small bit is very little, so there is no incentive for it to fly off away from the collet. (a spinning top doesn't leap away like a missile).

Greg J Sun 07 December 2008 11:24

Thanks Gerald,

I'll start expanding my comfort zone. :)

And reporting results.


All times are GMT -6. The time now is 11:59.

Powered by vBulletin® Version 3.8.3
Copyright ©2000 - 2019, Jelsoft Enterprises Ltd.