Hello Guest it is May 23, 2019, 03:36:24 PM

Author Topic: Need some advice!  (Read 1620 times)

0 Members and 1 Guest are viewing this topic.

Need some advice!
« on: April 22, 2016, 08:35:52 PM »
I am trying to cut 1\2 thick baltic birch plywood all in one pace. I am able to do it with my feed rate at 30in/sec and my RPMs at 2700 without breaking the bit but it just seems to have a little bit of burn marks. Here is the link to the bits that I use http://www.amazon.com/HQMaster-Carbide-Router-Acrylic-Hardwood/dp/B010NI39WO. I am trying to do this because it seem to get less blow out and burs when you only do one pass. This will save a tone of time with sanding afterwards. So the question is if I got a 3 or 4 flute bit would I be able to do this much easier? Any bit suggestions?
Re: Need some advice!
« Reply #1 on: April 23, 2016, 02:23:38 AM »
You are trying to cut 1/2 thick, with a 1/8" bit, at 30in/sec (probably 30"/min!!!) With a spindle running at 2700 rpm

I am not surprised....

Normally the recommended cutting depth per pass is 1/2 the bit diameter maximum!

Normally this is too deep for some machines because of machine ridgidity.

Key to successful cutting.... Stick to recommend chipload, and adjust depth of cut relative to machine rigidity.

Have a look at this PDF

Basically for a 1/8" cutter the chipload should be about 0.003/0.004"/tooth  (start with the 0.003"/tooth as birch is a hardwood)

If all your spindle will do is 2700rpm, then your feedrate is

0.003 x 2 (no of teeth on tool) x 2700 (rpm) = 16.2 in/min feedrate..... At a max depth of cut of 1/2 tool diameter (1/16")

If you want to do 1/2" in one pass.... You will need a 1" cutter and a very rigid machine.

I don't know how well it will work with plywood, but you could always try adding a finishing pass at full depth, the problem you have is that your tool is not very ridgid.... Being 1/8" dia and plywood not being the smoothest material as the grains are opposed..... But for this you look at the cutting face....
Say you have a 1/8" tool, and the recommended cut depth is 1/16", the cutting face area is 1/8" x 1/16" = 1/128" square, intended DOC = 1/2".... Therefore 1/128 / 1/2 (more correctly 2/128)  = maximum finishing cut of 1/64".... Which is not much.... Suggestion.... You need a larger diameter more rigid tool...

More flutes will increase your feedrate.... But not the depth of cut (DOC).... Only a bigger tool will do that (with a more ridgid machine that you probably don't have)

If you could use a 1/4" cutter at 2700 rpm, your finishing cut at full depth would be better.... (1/16")

And your feedrate would be 24.3"/min at a doc of 1/8".... But if your machine has ridgidity issues you may need to reduce this given you were using 1/8 cutters. And then proportionally adjust your finishing cut at full depth (1/2").

Also look at better cutters (onsrud for example) as you may get better chipload as you won't be guessing it ( they publish specific tables for tools.... And technical support is very good... Just ask the question and they will walk you through it... I know as I was failing to cut aluminium with one of their cutters (3/8", 1/8 dia cutter)


« Last Edit: April 23, 2016, 02:37:23 AM by robertspark »

Albert Einstein ― “If you can't explain it to a six year old, you don't understand it yourself.”

Offline RICH

  • *
  •  7,331 7,331
    • View Profile
Re: Need some advice!
« Reply #2 on: April 23, 2016, 06:50:20 AM »

You will find rather standard / similar charts and info as a that posted  in reply #2 for metal and the basis is from research done
many years ago. The info is a good reference point to start from. I have never found research based info for wood cutting. Wood and plywood have what I would call "non- standard" characteristics as the machinability can vary a lot even for a specific wood.

Burning comes from heat caused by friction. Adjust the way you machine the wood ( which includes the cutter ) and you can greatly reduce the condition.

So no use rambling on.......... test and adjust accordingly for what you are doing.


Offline ger21

  • *
  •  6,233 6,233
    • View Profile
    • The CNC Woodworker
Re: Need some advice!
« Reply #3 on: April 23, 2016, 01:05:19 PM »
Since this an X Carve, I'm going to assume that you are running at 27,000 rpm, not 2700. And 30ipm, not 30"/sec.

Couple things that will help.
1) Use a downcut spiral, it will cut cleaner.
2a) Lower your rpm if you can, to  12,000-13,000
2b) Increase feedrate to 100-125 ipm
3) Make 4 passes of 1/8" depth per pass, leaving .015" for a full depth finish pass

2010 Screenset

JointCAM Dovetail and Box Joint software
Re: Need some advice!
« Reply #4 on: April 23, 2016, 05:29:35 PM »
Thanks guys! This helped out a ton! Ill have to play around on it to see what works. Ger21 yeah it is 27,000 rpms and 30ipm. The final pass wounds like a really good idea!