Feeds/Speeds/and drilling pilots?

Post general information and questions relating to Cut2D in this Forum.

Feeds/Speeds/and drilling pilots?

Postby ironspider » Thu Apr 25, 2019 2:36 am

Greetings all! I just purchased Cut2D Pro and this is my first post. I have been watching the tutorial videos and now that my CNC is on the way (A CNC Router Parts PRO4824 with their spindle package (3HP, 8,000 - 24,000 RPM) I'm starting to get into starting out on my actual projects in the software. I have come to the section where I'm making my tool crib and setting feeds and speeds for my work. Many years ago I bought that G-Wizard software from CNCCookbook and was using that to determine feeds and speeds but I thought I would bring what I've got here and get your opinions/advice or flat out "whatever you do, don't do that!" I'm excited to get cutting but I'm also looking to avoid mistakes by looking to the helpful community.

So, my situation is that I will be doing two-sided machining on 1/2" Baltic Birch plywood with the aforementioned machine. I will be doing pocket and profiles of course but I also will be doing drilling of a a lot of 1/8" pilot holes that go about 1/4" deep. I was hoping to post the bits I've purchased so far and what the G-Wizard spit out for a workable feed and speed for this plywood and see if it looks good? And then I'd like to ask about the pilot holes.

Whiteside RD1600 Solid Carbide Downcut Spiral. 1/8" CD, 1/4" SH, 1/2" CL (for pocketing and profiles)
Pass Depth: 0.0625", Stepover .05 (40%), Spindle speed: 18,153, Feed Rate: 108 inch/min, Plunge Rate: 53 inch/min

Whiteside RD2075 Solid Carbide Downcut Spiral. 1/4" CD, 1/4" SH, 3/4" CL (for pocketing and profiles)
Pass Depth: 0.125", Stepover .1 (40%), Spindle speed: 18,153, Feed Rate: 137 inch/min, Plunge Rate: 67 inch/min

As for the pilot holes, I want to do 1/8" pilots about 1/4" deep. I was planning on just peck drilling with the RD1600 but then I was reading in a lot of places that you never want to use a downcut bit for pilot holes since that could start a fire since the chips have nowhere to go? So should I just get the upcut version of the RD1600 (the RU1600) to do those with? Or would I be okay by doing very small pecks with the RD1600 (thus avoiding buying another bit and having to do another manual tool change)? Again, these pilots are going to be 3/8 at the absolute max. And should the spindle speed and plunge be different on this bit for a peck drilling toolpath? Or can I just use the same spindle speed and plunge?

Thanks in advance, I'm excited to be part of the Vectric community!
ironspider
 
Posts: 12
Joined: Tue May 28, 2013 9:23 pm
Location: Los Angeles, California
Model of CNC Machine: CNCRouterParts PRO4824

Re: Feeds/Speeds/and drilling pilots?

Postby wb9tpg » Thu Apr 25, 2019 12:33 pm

I use Amana Tool 51692 for 1/4" holes. They have other sizes available and you can see them on this webpage below. You can thank me later

https://www.amanatool.com/51692-high-pe ... -mill.html
wb9tpg
Vectric Apprentice
 
Posts: 81
Joined: Tue Sep 04, 2018 2:49 pm
Model of CNC Machine: Shapeoko 3 XL

Re: Feeds/Speeds/and drilling pilots?

Postby ger21 » Thu Apr 25, 2019 2:22 pm

Your RPM is too high with the 1/4" bit. I'd lower it to 12,000-14,000. And I'd cut 3/16-1/4" depth per pass.
I prefer to ramp in at cutting speed.

For drilling, I'd get a short length 1/8" drill bit. You can use the downcut, but you'll likely get some burning. Don't peck, just do it in one shot, at 100-150ipm. Whether you use the downcut or a drill bit.
Gerry - http://www.thecncwoodworker.com
ger21
Vectric Wizard
 
Posts: 1447
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA
Model of CNC Machine: Custom DIY

Re: Feeds/Speeds/and drilling pilots?

Postby ironspider » Fri Apr 26, 2019 4:01 pm

So if I went with the two-flute 1/8" version of that (which is model 51650) for drilling what RPM and Plunge Rate would I be shooting for? I looked at the PDF they have on the page and my rough calculations (it doesn't list wood as a material so I just picked a number in the plastics section for SFM[420]) came out to an RPM of around 13,000 with a "Feed Rate IPM" of 78 (which I assume I divide by 60 to get Vectric's Plunge Rate in inch/sec?) of 1.3

Is that in the ballpark of what you set it for on plywood?

Also, I thought I read that 4 flute and coated bits were more for metal machining, not wood?

wb9tpg wrote:I use Amana Tool 51692 for 1/4" holes. They have other sizes available and you can see them on this webpage below. You can thank me later

https://www.amanatool.com/51692-high-pe ... -mill.html
ironspider
 
Posts: 12
Joined: Tue May 28, 2013 9:23 pm
Location: Los Angeles, California
Model of CNC Machine: CNCRouterParts PRO4824

Re: Feeds/Speeds/and drilling pilots?

Postby ironspider » Fri Apr 26, 2019 4:13 pm

Thanks for the reply Ger, I think I bought your Mach3 2010 screenset like 6 years ago! :) Does your bit about "ramp in at cutting speed" mean your Vectric Plunge Rate is the same as the Feed Rate and you select "Ramp Plunge Moves" when generating toolpaths in the software?

And is there some formula to calculate the "Distance" amount for "Ramp Plunge Moves"? It seems to be set to 1" by default but I didn't know if there's some way to calculate a better number?

Thanks all!


ger21 wrote:Your RPM is too high with the 1/4" bit. I'd lower it to 12,000-14,000. And I'd cut 3/16-1/4" depth per pass.
I prefer to ramp in at cutting speed..
ironspider
 
Posts: 12
Joined: Tue May 28, 2013 9:23 pm
Location: Los Angeles, California
Model of CNC Machine: CNCRouterParts PRO4824

Re: Feeds/Speeds/and drilling pilots?

Postby ger21 » Fri Apr 26, 2019 4:58 pm

1) Change the feedrate to ipm for your tools, so you aren't converting to ips.

Yes, set plunge rate same as feedrate.

Ramp distance may depend on what you are doing but 1"-2" should be plenty.
Gerry - http://www.thecncwoodworker.com
ger21
Vectric Wizard
 
Posts: 1447
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA
Model of CNC Machine: Custom DIY

Re: Feeds/Speeds/and drilling pilots?

Postby ironspider » Sat Apr 27, 2019 2:17 am

Okay Ger, followed some of your suggestions and recalculated. But I'm still not sure what my spindle speed should be on the drill bit below? (8,000rpm is the lowest my spindle will go). How does this look?

Whiteside RD1600 Solid Carbide Downcut Spiral. 1/8" CD, 1/4" SH, 1/2" CL (for pocketing and profiles)
Pass Depth: 0.0625", Stepover .05 (40%), Spindle speed: 14,000, Feed Rate: 87 inch/min, Plunge Rate: 87 inch/min
Note: Ramp in from 1.5"

Whiteside RD2075 Solid Carbide Downcut Spiral. 1/4" CD, 1/4" SH, 3/4" CL (for pocketing and profiles)
Pass Depth: 0.1875", Stepover .1 (40%), Spindle speed: 14,000, Feed Rate: 77 inch/min, Plunge Rate: 77 inch/min
Note: Ramp in from 1.5"

McMaster-Carr 2956A43 Short-Length Carbide Drill Bit, 1/8" Diameter, 1/8" SH, 1/2" Max Drill Depth (for 1/4" deep pilot holes)
Spindle Speed: ????? Plunge Rate: 125 inch/min
Note: Pass Depth .25" no peck drilling
ironspider
 
Posts: 12
Joined: Tue May 28, 2013 9:23 pm
Location: Los Angeles, California
Model of CNC Machine: CNCRouterParts PRO4824

Re: Feeds/Speeds/and drilling pilots?

Postby ger21 » Sat Apr 27, 2019 11:02 am

For drilling, keep the rpm as low as possible.
With my SuperPID controlled router, I drill at 5,000 rpm.
Gerry - http://www.thecncwoodworker.com
ger21
Vectric Wizard
 
Posts: 1447
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA
Model of CNC Machine: Custom DIY

Re: Feeds/Speeds/and drilling pilots?

Postby ger21 » Sat Apr 27, 2019 11:09 am

When you lowered the RPM to 14,000, the feedrates should have stayed the same.

You can easily cut at 150-200ipm at 14,000 rpm.

And why are you cutting faster with the smaller bit? With an 1/8" bit, I'd make 1/8" deep passes. 1/8" deep is barely removing any material, and 1/8" bit's are tougher than you may think.

A couple things about feeds and speeds.

1) Most people can easily cut deeper and faster than they are used to, based on all of the posts that I read.
2) Sometimes you have to cut shallower, or slower, to get the quality of finish you are looking for.

It's not an exact science when working with wood. Grain direction, species, and density can all play a role, and can vary even in a single piece of wood. Sometimes you need to work with the wood.
Gerry - http://www.thecncwoodworker.com
ger21
Vectric Wizard
 
Posts: 1447
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA
Model of CNC Machine: Custom DIY


Return to Cut2D - General

Who is online

Users browsing this forum: No registered users and 5 guests