Feeds and Speeds

This forum is for general discussion regarding VCarve Pro

Feeds and Speeds

Postby jib2 » Wed Jan 27, 2016 1:51 pm

Has anyone used this product?

http://www.cnccookbook.com/CCGWizardv1. ... tware.html

It appears to be mainly for machine metal so I was wondering if anyone has done the trial version and if it has calculations for various types of wood. If so, what is your opinion of the product is it worth the dollars? It seems that optimizing speeds and feeds would be very beneficial.

If not does anyone have suggestions or is their a well populated tool database that can be shared with some description of different wood types?

I know this maybe a stretch however, I have very little machining background and I'm always reading and looking for something to help me understand what is optimum.

Thanks, look forward to your responses and or suggestions.
jib2
Vectric Apprentice
 
Posts: 57
Joined: Mon Nov 03, 2014 12:46 am
Model of CNC Machine: Laguna CNC

Re: Feeds and Speeds

Postby Adrian » Wed Jan 27, 2016 2:11 pm

There are quite a few posts about it on the forum and lot of people seem to swear by it.

Personally I wouldn't bother for machining wood. The feed rate calculations are very simple and there are loads of charts about (I use this one - https://www.vortextool.com/images/chipLoadChart.pdf although your own tool supplier should have one available).

The important thing to remember is that any chipload calculation is just a starting point. You need to look at the quality of the cut and listen to the cutting to work out the optimum settings. Even then it's still just a ballpark figure as, unless you're doing lots of long straight cuts, the machine will have to slow down for corners and on shorter segments may never get to the programmed speed in the first place.

Not to mention that wood is a variable material so what works for one sheet might not work exactly the same for the next plus the performance of the cutting bit will change as it wears.

All a very long winded way of saying that it's something you learn as you go along. It doesn't take long to get proficient.
User avatar
Adrian
Vectric Archimage
 
Posts: 8606
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Feeds and Speeds

Postby FastFarmer » Wed Feb 03, 2016 10:03 pm

I use this for EVERY job. Not only does it maximise my cutter efficiency with the correct tooth load, it ensures I get the surface finish I seek.

For most jobs, I have found it's best to drop the plunge rate to the next lowest recommendation.

However, even though I think it does a great job, I loathe the subscription type service for payment each year and it's nothing short of a TOTAL rip off. Like 95% of programs, I will always prefer to pay once and then pay for upgrades.
FastFarmer
Vectric Apprentice
 
Posts: 49
Joined: Tue Apr 09, 2013 9:26 am
Model of CNC Machine: BF-30 mill and 360 x 100 lathe

Re: Feeds and Speeds

Postby scottp55 » Wed Feb 03, 2016 11:00 pm

I'm with Adrian,
Feeds change depending on the file and what you're trying to do, which species,which machine, the exact cut of the bit and how sharp it is.
You'll learn your machine fairly fast and learn what the cut quality you need sounds and feels like and mod your database.
Personally like to do new bits in Hard Maple for a basis point, and then I know how much to mod roughly by Janka hardness.
Too many personal decisions for quality/speed to be a universal best.
Only hardwoods here, but usually start about 60,30,12-14K and keep a hand on the VFD while watching Chips, Then incrementally increase feed/speed proportionately until quality of cut falls off and the decrease both 10%.
So long as the bit stays room temp or very slightly warm to the touch, AND the cut quality is good...I'm happy.
2 cents from a basic newbie,
scott
User avatar
scottp55
Vectric Wizard
 
Posts: 2406
Joined: Thu May 09, 2013 11:30 am
Location: Kennebunkport, Maine, US
Model of CNC Machine: Shopbot Desktop 5.5"Z/spindle/VCP9

Re: Feeds and Speeds

Postby kaetamer » Thu Feb 04, 2016 1:09 am

Any advice on chipload numbers for vbits? Does chipload even matter? I carve at about 20 ipm , 14100rpm with a 2 flute 30 degree vbit with a tip diameter of .005. Chipload calculates out to .0007. Seems like a nonsensical number.
Any thoughts?
Scott
kaetamer
Vectric Apprentice
 
Posts: 24
Joined: Mon May 12, 2014 3:10 pm
Model of CNC Machine: CNCRP Pro 4824

Re: Feeds and Speeds

Postby JoeM » Thu Feb 04, 2016 2:02 am

kaetamer wrote:Any advice on chipload numbers for vbits? Does chipload even matter? I carve at about 20 ipm , 14100rpm with a 2 flute 30 degree vbit with a tip diameter of .005. Chipload calculates out to .0007. Seems like a nonsensical number.
Any thoughts?
Scott

That # only makes sense if the .005" wide part of the bit is the only thing touching the wood.
JoeM
Vectric Craftsman
 
Posts: 284
Joined: Fri May 29, 2015 1:51 am
Location: Arizona
Model of CNC Machine: Shop-Made Router

Re: Feeds and Speeds

Postby kaetamer » Thu Feb 04, 2016 4:59 pm

JoeM wrote:
kaetamer wrote:Any advice on chipload numbers for vbits? Does chipload even matter? I carve at about 20 ipm , 14100rpm with a 2 flute 30 degree vbit with a tip diameter of .005. Chipload calculates out to .0007. Seems like a nonsensical number.
Any thoughts?
Scott

That # only makes sense if the .005" wide part of the bit is the only thing touching the wood.

Okay, I see your point. I usually carve somewhere around .04" deep, which roughly equates to the bit diameter in contact with the wood at that depth to be about .0265". I haven't found a table that lists chipload for bits of that diameter, hence my question. Obviously, the point of this is to maximize cutting speed without breaking bits constantly. At my current settings bits generally dull before they break but I wonder if I'm cutting too conservatively. Blind experimentation with feed rates and RPM would likely sacrifice many bits and yield little useful info.
Thanks for your input.
Scott
kaetamer
Vectric Apprentice
 
Posts: 24
Joined: Mon May 12, 2014 3:10 pm
Model of CNC Machine: CNCRP Pro 4824

Re: Feeds and Speeds

Postby scottp55 » Thu Feb 04, 2016 5:08 pm

Scott,
For a similar bit I use with similar cut depth,depending on wood, try 45-60 IPM at between 16-17K.
May be a good starting point.
scott
User avatar
scottp55
Vectric Wizard
 
Posts: 2406
Joined: Thu May 09, 2013 11:30 am
Location: Kennebunkport, Maine, US
Model of CNC Machine: Shopbot Desktop 5.5"Z/spindle/VCP9

Re: Feeds and Speeds

Postby Adrian » Thu Feb 04, 2016 5:28 pm

You don't need to break bits when experimenting with faster feeds or slower RPMs. Just take it incrementally from where you are now and increase the feed rate or slow the RPM's until the finish starts to deteriorate and/or the machine is obviously struggling. You'll only break bits if you make big changes in one go.

Don't forget to take into account the type of job you will be doing as well. I use different settings for cabinet jobs compared to lettering jobs even though the material and bit is the same. The length of the straight runs is totally different so the feed rate set for the cabinets is never reached on the lettering meaning the RPM's are far too high and causing bit wear.
User avatar
Adrian
Vectric Archimage
 
Posts: 8606
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Feeds and Speeds

Postby FastFarmer » Thu Feb 04, 2016 8:52 pm

Hahaha. Well wood is about the only material I never cut, but its funny you guys are recommending guess work.

Even for a hobby guy where perhaps the dollar is tight, I would have thought guessing isn't really an acceptable practice.
FastFarmer
Vectric Apprentice
 
Posts: 49
Joined: Tue Apr 09, 2013 9:26 am
Model of CNC Machine: BF-30 mill and 360 x 100 lathe

Re: Feeds and Speeds

Postby Adrian » Thu Feb 04, 2016 9:24 pm

It isn't guessing. It's using the chipload calculations to get a starting point and realising that those calculations are only that, a starting point. Unless you can put in the exact condition of the bit, your acceleration/deceleration settings, spindle weight, maximum straight line cut of the job, tightest radius and several other factors no program is going to give you the exact cutting parameters. The smaller the machine the closer its likely to be which is why the various calculator programs work well for the smaller milling type machines. An 8' x 4' machine cutting sheet materials at 800+ ipm is a different ball game.

I cut a lot of plastics as well as various recycled products and I follow the same practises for those as well. It's even more important in plastic as the wrong settings will cause remelting onto the bit.

Getting the settings just right can drastically increase the life of the bit and that's good for hobbyists and production shops as carbide is expensive.
User avatar
Adrian
Vectric Archimage
 
Posts: 8606
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Feeds and Speeds

Postby IslaWW » Fri Feb 05, 2016 12:29 am

Adrian is spot on. However I take exception to the introduction of the term "guess work". Wood is both easier and harder to cut than most metals. Easier to cut, possibly harder to cut well.

The reason for ambiguous feeds and speeds and the use of the term "starting point" is that wood does not have anywhere near the consistency of metals. Metals are graded as to hardness, temper, etc. and as such are much more predictable. Wood on the other hand will vary from one board to the next, even having areas that are 50% harder or softer than the norm within a small area. Wood density is not consistent, nor are the grain patterns or moisture content. A file that you ran on Friday may require a feedrate adjustment on Monday due to ambient humidity changes. You may have to adjust for each different board.

I have cut both metals and wood, and to tell the truth, most metals are easier. I can usually just take the feeds and speeds out the book and cut away. Wood, not so much. An experienced user with a trained ear or eye to the cutpath can make proper adjustments to achieve high quality cuts. Call it guesswork if you wish, but the principles of chipload must be applied to an ever changing material.
Gary Campbell
CNC Technology & Training
The Ultimate Woodworking Machine
GCnC411 (at) gmail.com
User avatar
IslaWW
Vectric Wizard
 
Posts: 1133
Joined: Wed Nov 21, 2007 11:42 pm
Location: Marquette, MI, USA
Model of CNC Machine: The Ultimate Woodworking Machine

Re: Feeds and Speeds

Postby tomgardiner » Fri Feb 05, 2016 2:25 am

One thing that has not been mentioned with respect to feeds and speeds is what is holding the work. Often the depth of cut or feedrate has to be adjusted if your workpiece cannot be held as firmly as you may want. If I am cutting sheet goods with the vacuum pump I may back off the feedrate when working small parts. Aluminum parts screwed to the spoilboard are the worst for vibration and sends me running for the controller. I must look into a low profile machinists vise soon.

Tom
tomgardiner
Vectric Craftsman
 
Posts: 294
Joined: Thu Oct 02, 2014 1:49 pm
Model of CNC Machine: FMT Patriot 4 x8

Re: Feeds and Speeds

Postby scottp55 » Fri Feb 05, 2016 3:10 pm

+1 Adrian and Gary!
Last I knew, metal didn't have knots and endgrain, or Curly and Quilted patterns:)
scott
User avatar
scottp55
Vectric Wizard
 
Posts: 2406
Joined: Thu May 09, 2013 11:30 am
Location: Kennebunkport, Maine, US
Model of CNC Machine: Shopbot Desktop 5.5"Z/spindle/VCP9

Re: Feeds and Speeds

Postby TReischl » Sat Feb 06, 2016 5:27 pm

These wood cutting feed/speed discussions always interest me.

From Onsrud about wood:

Feed Rate (IPM) = RPM x # of cutting edges x chip load

What does all that mean?

A router that runs permanently at 25K for a starting point and about a .25 cutter:

Feed Rate = 25000 * 2 flutes * .007 chipload per tooth = 350 IPM

Let's go to the low end of a variable speed router:

Feed Rate = 12000 * 2 flutes * .007 chipload per tooth = 168 IPM

Sooo, unless you can really slow down your spindle, it is apparent that most cuts need to be done at a fairly high feedrate. The problem is that a lot of the hobbyist machines (which is what I have) do not perform well at 300+ IPM. Things like inertia get in the way.

However, I have cut as high as 800 IPM on mine, posted a video of it doing that some time ago. Here it is again:

https://www.youtube.com/watch?v=Pt8n43_YRjI&list=UUDVvMj8gloyBSn18tqqVgrw&index=23

That cut is with a .5 dia end mill that was far from brand new. Edit, my bad, that cutter was .25. and it is sticking out way past where it should be.

My feeling is that most people are running their machines way too slow. I will freely admit that includes me. I am not keen about a machine rapiding around at 800 IPM, things happen awfully fast at those feedrates. Since I am no hurry, most of my cutting these days is done at around 200 IPM .
http://www.tedreischl.com

Low Profile CNC Router Vise
User avatar
TReischl
Vectric Wizard
 
Posts: 2091
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X8 RP 2010 Screenset


Return to VCarve - General

Who is online

Users browsing this forum: Google [Bot] and 31 guests