Hey all, was wondering if someone can explain this for me, or lead me somewhere, where this is explained in plain english?

Is the chip load only dependant on the feedrate, RPM, and number of cutting surfaces (flutes)? I saw a formula online that states that

chip load = feedrate / (RPM * [number of flutes])

The formula does not take into account the bit size? The reason I ask is that I know intuitively that with smaller bits, I should increase the RPM. But in theory, should I increase the RPM so that the outer edge of the bit matches that of a larger bit that I know I cut successfully with?

For example, I'm using a 1/4" spiral-o-flute upcut bit, at about 15K RPM, and 40-45ipm, at .080 depth. Does this mean that I should run a similar 1/8" bit at 30K RPM and keep the feedrate constant, or keep the same RPM, and lower the feedrate by half? Is it directly proportional, as the formula suggests, or am I missing something?

I do not use multi-flute bits to do pocketing in aluminum because they always seem to gall with the high RPM, but I do use them for cleanup passes where there is a place for chips to clear easily.

2. Is the chip load only dependant on the feedrate, RPM, and number of cutting surfaces (flutes)?
Actually, the feedrate, rpm and # of flutes are dependent on the chip load.
The tool manufacturer should tell you what the recommended chip load should be. You then adjust rpm and feedrate to obtain that chip load. Be aware that it can be difficult to obtain a proper chip load on a homebuilt machine, especially with larger tools, as proper chiploads can require large cutting forces and high spindle power. Taking shallower cuts can alleviate these issues, but cause more wear on the tip of the tool.

As bit diameter increases, so does chip load. But it's not proportional. Chip load increases gradually as diameter increases.

The formula does not take into account the bit size? The reason I ask is that I know intuitively that with smaller bits, I should increase the RPM. But in theory, should I increase the RPM so that the outer edge of the bit matches that of a larger bit that I know I cut successfully with?
No.

For example, I'm using a 1/4" spiral-o-flute upcut bit, at about 15K RPM, and 40-45ipm, at .080 depth. Does this mean that I should run a similar 1/8" bit at 30K RPM and keep the feedrate constant, or keep the same RPM, and lower the feedrate by half? Is it directly proportional, as the formula suggests, or am I missing something?
The chipload for a 1/8" tool is similar to that of a 1/4" tool, so if you double the rpm, you need to double the feedrate. You don't keep increasing feedrate as bits get smaller. It's usually the opposite. The larger the tool, the faster you can go, because the larger tools are stronger.

Not sure with aluminum, but with wood, you should use the lowest rpm that gives an acceptable surface finish. The higher the rpm's, the more heat that is generated. Heat is the enemy of tooling. So lower rpm's generally are better.
As you decrease rpm, though, at some point, the finish quality will deteriorate.

Bottom line, is to follow the manufacturers chip load whenever possible. It's OK to use your gut feeling for rpm, but the feedrate needs to be correct for whatever rpm you choose, to achieve the recommended chip load.

3. Originally Posted by ger21
Actually, the feedrate, rpm and # of flutes are dependent on the chip load.
The tool manufacturer should tell you what the recommended chip load should be. You then adjust rpm and feedrate to obtain that chip load. Be aware that it can be difficult to obtain a proper chip load on a homebuilt machine, especially with larger tools, as proper chiploads can require large cutting forces and high spindle power. Taking shallower cuts can alleviate these issues, but cause more wear on the tip of the tool.

As bit diameter increases, so does chip load. But it's not proportional. Chip load increases gradually as diameter increases.

No.

The chipload for a 1/8" tool is similar to that of a 1/4" tool, so if you double the rpm, you need to double the feedrate. You don't keep increasing feedrate as bits get smaller. It's usually the opposite. The larger the tool, the faster you can go, because the larger tools are stronger.

Not sure with aluminum, but with wood, you should use the lowest rpm that gives an acceptable surface finish. The higher the rpm's, the more heat that is generated. Heat is the enemy of tooling. So lower rpm's generally are better.
As you decrease rpm, though, at some point, the finish quality will deteriorate.

Bottom line, is to follow the manufacturers chip load whenever possible. It's OK to use your gut feeling for rpm, but the feedrate needs to be correct for whatever rpm you choose, to achieve the recommended chip load.
Cool thanks... For wood is normally not an issue because I have a pretty good feel for the feedrates and RPMs; being a cabinetmaker/woodworker my whole adult life, I can usually "hear" when I'm making good cuts, or the bit is not working enough/too much.

As for the aluminum, I've tried with some success to apply what I've learned from past errors (mainly breaking bits!). After looking at Amana's site, they recommend, for 1/4" spiral-o-flute bit, 120IPM at 18000RPM, and 1/4" depth! I don't think I can come close with my machine, so I picked a slower speed, 100IPM, and made experiental cuts in .015" incrememts. To my surprise, I was able to get to .075" and still keep a relatively burr-free edge. This left a somewhat rough but flat finish on the bottom. I tried .090" but the cut was not as clean.

At these speeds I'm not getting as clean a finish as I would like, though my goal was to see how close I could get to the recommended speeds with what I have.

I also experimented using 2 and 4 flute bits for a finishing or cleanup pass. I found that the 2 flute areound 50IPM and .005" depth gave me the bext mix of finish and speed. I tried the 4 flute at 100IPM+ and .005" depth, and though it did look shinier, I don't know if I want to run the machine that way...

4. I guess I was asking myself the same few question about feedrate and chip load and I was unsatisfied of only finding the same unfullfilling formula that you stated. You can clearly see that yes something is missing.

so after 2 days or research for something a bit more scientific I found what I was looking for. The Formula for calculating the chip load per tooth value. which then you can plug into your rpm and number of tooth which will give you the correct feed rate you should be using.

so here is the link with great technical info.
http://www.kennametal.com/images/pdf...foFormulas.pdf

the formula is at the bottom of page 1.
But there is something missing, and it is the dept of cut which also affect the equation.

If you refer to the tables Chiploads | Feeds and Speeds | Metal | Plastic | Composite | | LMT Onsrud

DEPTH OF CUT:
1 x D Use recommended chip load
2 x D Reduce chip load by 25%
3 x D Reduce chip load by 50%

I am sure there is something a bit more advanced than this but right now I am satisfied. Of course this doesn't tell you if the nuber you are getting at the end is correct of not. I saw some chart around with typical feedrate for metals, nothing for wood yet. but just comparing with the onsrud tables if you are getting values more of less in synch it means you got the chip load factor correct.

I know that my cnc can't even approach the calculated feedrate anyhow unless I would be using a 2 turn per inch acme rod.

hope this help, I saw a few other post looking for something like this.

5. I've continued researching feed rate, deflection, forces and I've even found formulas on harmonics and tool shatter speed.

I'm doing some all-in-one excel spreadsheet to check this out and if I come up with something working I'll post it here.

I had to write to one of the website I refered above since their equation bugs me for some conditions like in the case of profiling the total width of the bit, they should comeback to me eventually....

6. Lou and Base,
After extensive research this website probably has the best collection of stuff around.

CNC Cookbook: Software and Information for Machinists

He is selling a calculator but he also has some very good information including information on chip thinning and deflection.

I am still evaluating his software but think it deserves a look.

Dave

7. Dave, does G Wizard cover wood, or just metals?

8. Gerry,
The latest version has several material entries for wood. I think it was MDF, hardwood, plywood and softwood.
I am still working on my decision on how good the calculator is. But I can say that that support material is very complete and shows that Bob has spend a lot of time researching the material.
I have been doing some testing on aluminum on my little CNC mill, but now fixing some deficiencies in the Mill then have to rerun the test

Dave

9. I had a look at Gwizard last week, very nice indeed and yes it got wood data as well and also tool bit references which is very handy.

My speadsheet is based on the theory I listed below in the post and it matches what Gwizard gives. So what else do I need more for now? nothing! I'm happy, I found what I was looking for and it is all there for people to grab.

If people are willing to pay for Gwizard, I can't argue! but I've got a hard time to pay for something that is free and that I can match with a simple spreadsheet unless I had too much money or I was running a business, not for a simple home made cnc project.

Maybe one day I'll take the time to code something and release some opensource apps.

10. Base,
I am sure there are many people that would like to have a copy.
Dave

11. there is a good spreadsheet here (not mine)

12. Originally Posted by Base
I had a look at Gwizard last week, very nice indeed and yes it got wood data as well and also tool bit references which is very handy.

My speadsheet is based on the theory I listed below in the post and it matches what Gwizard gives. So what else do I need more for now? nothing! I'm happy, I found what I was looking for and it is all there for people to grab.

If people are willing to pay for Gwizard, I can't argue! but I've got a hard time to pay for something that is free and that I can match with a simple spreadsheet unless I had too much money or I was running a business, not for a simple home made cnc project.

Maybe one day I'll take the time to code something and release some opensource apps.
I think a spreadheet alone would suffice. I've posted somewhere else my revised feeds and speeds, and how to adjust for different bit diameters and number of flutes as well, as far as aluminum is concerned... I think hardwoods and softwoods are too broad a generalization, since they all cut differently. Heck, basswood is considered a hardwood but you can plow through it like a hot knife through butter. Douglas fir is a softwood, but some pieces can be harder than some hardwoods. Oak can tear out like crazy, while you may never get tearout with alder. Some woods are gummy, some are oily, some are dry, etc.

As important as feeds and speeds are, using the right bit can make all the difference. Believe it or not, there are specialized bits for both softwoods and hardwoods and composites and laminates. A bit that cuts clean in one material may be too aggressive or not aggressive enough. Also, I use a few bits intended for hand-held routers (like a lot of us do) but one must consider that their flute designs are anti-kickback and have a limited radial depth of cut. The flutes on CNC-specific bits are more open and can be pushed more aggressively. In fact, for woods that are prone to chip and tear, it may be better to use a regular router bit, since it won't take as big a "bite" so to speak as a CNC router bit, but a lot has to do with spindle speed, power, and the ridgidity of the machine.

Page 1 of 2 12 Last