Facing Operation Feeds/Speeds

[GeorgeIoak]

Hello everyone, 1st post and new user so try to be kind!

I joined a local hackerlab that has a PRS Alpha with a 2KW spindle. I've only be on the machine 3 times and I'm still getting the feel for things.

To help me learn a little more about feeds and speeds I've downloaded GWizard (http://www.cnccookbook.com/CCCNCSoftware.html) and using that to compare against some notes and posts that I've read. I purchased an Infinity Tools Planar bit (52-506 (http://www.infinitytools.com/1_2-Shank-Mega-Dado-Planer-Bit-2-CD-1-CH/productinfo/52-506/)) which is a 2" bit with 4 flutes.

My question is this, in reading the posts that I can find about face milling I read most people are running at over 10k RPM. Using GWizard it calculates I should be running at 3075RPM, 38.261 IPM, for a cut depth of 0.01 and width of 0.8.

This yields a chip load of 0.0039 which seems to be in the window I find for other bits. I plan to initially use MDF and then switch to Cedar.

Any feedback and/or guidance would be greatly appreciated!

Thanks,
George

[Brady Watson]

12,000 RPM, 5-6 IPS, .025 DOC. Start there for MDF. Keep adding more speed until cut quality degrades, then back off, or raise RPM until quality is restored.

4-flute tools are generally for low RPM spindles, typically found on milling machines. Use a 2-flute tool for routing because you cannot run @ 3,000 RPM - no power and VFD will not go below 5,000 on most newer machines. You also want a 2-flute to give additional chip clearance when machining woods. Using a 2" tool at low RPM will stall the spindle. Keep the RPMs up...it's like a 2-stroke (router), not a diesel (milling machine).

My advise is always to jump in and do - rather than get caught up in analysis paralysis. This will build skills no book or reference sheet can teach you - especially when it comes to dealing with materials not on the list. The power of observation and your own deductions trump books and lists. You can start cutting just about any material at MS,2,1 @ 12,000 RPM. This is a general baseline number. Feather speed up or down and observe/listen to what the machine is telling you where it wants to be for a given material.

Watch the max RPM rating on the larger dia tools. They can fly apart if run too fast.

-B

[curtiss]

....Watch the max RPM rating on the larger dia tools. They can fly apart if run too fast.

Good advice... check my math but...

tip speed on a 2 inch bit at 20,000 RPMs is 153 mph.

4 inch bit @ 20k would be 307 mph....

[GeorgeIoak]

OK, thanks for the good general advice. I had already run a test piece with this bit on MDF but the surface had minor ridges between the passes. I think was probably do more to me not securing the board down enough rather than any settings.

That speed did seem rather slow and I wasn't sure what the minimum was for this unit. I don't think I've seen any posts where people go slower than 10k RPM so it made me nervous to just try that. Do you think this is a poor choice of a bit for face milling? The lab has an Onsrud 91-000 which is a 1.25" 2 "flute", but it was missing the last time I went so I decided to buy my own and I thought a 2" bit would be nice.

I played around with that calculator and changed the number of flutes to 2 from 4 but it still wants to run it at 3k rpm. It could be I'm just configuring the calculator incorrectly but I've tried several settings.

Most of the other bits I have are single or 2 flute and I have them set to run at 12k RPM and maybe ~3 IPS. When I enter parameters into that calculator for hardwood, 1/4" 2 flute bit, it says to run it at 18,000 RPM , 0.0336" DOC, and 62.178 IPM which doesn't seem to match what everyone else seems to be doing so maybe this calculator is goofy or it's a case of operator error!

[Brady Watson]

The calculator was designed for milling machine operations. Chipload is for maximum tool life in production routing situations. Running @ chipload is NOT in any way a reflection of the cut quality you will get by running it. It is only pegged to maximum tool life...and carbide lasts a long, long time. It is irrelevant for most jobs and users.

I would advise losing the calculator and proceed with cutting, making adjustments along the way. If it was just a matter of plugging in numbers and having it be all hucky duck, there would be absolutely no need for a CNC operator.

Lines are from improper hold down or the Z is out of square. Hold down is about 85% of the entire job of machining.

You can run the 4 flute. When that one dies, get a 2-flute. MCLS has 1.5" under $20; 2" under $30 IIRC. I run an Amana 2+2 insert that cuts beautifully.

Sorry, but all you are going to get is general advise. Without knowing the quality or density of the MDF, how the material is being held down and what you are doing precisely, it is impossible to give exact anything. This is a skilled craft where operator observation/correction is required if you want to approach professional results.

My advise still stands - keep cutting, testing and by using cut quality as a gauge, sneak up on your best edge. I've been cutting and training people to do this work professionally for 15 years. I have no interest in leading you astray.

-B

[GeorgeIoak]

Thanks for the honest and helpful reply. It's a pleasure dealing with people that actually know what they are talking about rather than people who just like to spout answers. I plan to get back on the machine later this week one night but was just trying to get some helpful guidelines to make sure I was heading in the right direction.

I know my hold down method wasn't the best so the lines are most likely from that. The MDF I'm starting with is just the cheap stuff from Home Depot so quality is not very good for CNC work. I figured it was better to practice on the cheap stuff before I move on up to more expensive material. Later this week I need to make a circular trim piece out of cedar for my house gable vent so I wanted to make all my major mistakes on this MDF project first.

Thanks again for the helpful advice.

[Brady Watson]

You're welcome & Welcome to the SB Forum.

Take your time, don't cut corners - and you'll do fine.

-B

[GeorgeIoak]

Thanks again for your advice. I went last night and made some more cuts and for the most part things went well using your recommendations. Can you point me to some videos or something that shows what happens with non-ideal feed rates and speeds? Of course worse case is easy to understand but I'm trying to get a feel for when to increase RPM and/or bump up the feed rate. I'm using Fusion 360 for my software and I'm not sure if it's because of the way it generates files or it's just typical but there are many VS commands in the file. If I issued a "SHIFT >" command the feed rate would increase but I think at the next VS command in the file it would get changed again so it was difficult to see the impact of changing the feed rate.

I've got a few other questions but I don't want to hijack my own thread so I'll probably start another post on those.

[barrowj]

You might also want to delve into the .sbp file to get an understanding of this. It's an easy "search and replace" command to change all of the VS parameters:

VS - Values for Speeds{XY Move Speed, Z Move Speed, A Move Speed, B Move Speed, XY Jog Speed, Z JogSpeed, A Jog Speed, B Jog Speed}

I use Aspire 8 and normally I only have MS commands which of course is easier to change.

MS - Move Speed Set{xy-Speed, z-Speed, a-Speed, b-Speed}

Unless you are using an ATC , I would remove all of the VS command and at the beginning of the file insert the MS command.

Joe

[GeorgeIoak]

I did poke into the .sbp file and saw those commands. I'm not sure if those are inserted from Fusion 360 because of a setting that I have selected so I may have to change a few things and compare .sbp files. It doesn't seem to me that you should need to change speeds in most cases so removing the VS commands and just using the MS as you suggested sounds like a good start.