CNC Tooling

[DampRobot]

Originally Posted by DonRotolo

DampRobot, 6 IPM is 1" in 10 seconds, or 0.1" per second. Just seems slow to me, but....

1. You're getting good results. Something must be right, eh?
2. What kind of depth of cut we talkin here? 0.1" or 1/2"? That matters...

Anyway, I keep looking at #1 above and concluding it's OK.

I remember vaguely that the tool moved about one tool diameter every two seconds (for a 1/4" tool) when we were cutting quickly. That gives a feed rate of 7.5 IPM, which squares fairly well with the 6-10 value I remember. I recall it seeming quite fast, but I guess it's all relative.

We have got results we're pleased with. We don't have to deal with anything as intensive as flood cooling, and we don't feel like milling something takes too long (setup and tool zeroing still dominates the time spent on the mill). With a 1/4" tool, we usually wouldn't cut anything thicker than 1/4" alu plate at that speed. Stuff on the 1/2" or larger scale we would use a larger cutter (1/2" or something) and probably even do in multiple passes, depending on the geometry and the tool. With 3/16" tools or smaller in 1/4" or even possibly 1/8" material, we'd take multiple passes too, just to be safe.

Since others have shared their advice about cutting faster (in the 20-60 IPM range), I'll definitely make a point of trying it. Cutting faster is always good, as is better tool life, etc. Since we do make good chips and cut quickly enough for our tastes at our current speeds, if we don't have success with the higher speeds, we'd be happy going back to what we're more familiar with.

Thanks to everyone for their experience and suggestions. I'll post again in this thread when I get a chance to experiment with the speeds on our mill.

[Mr. Mike]

Roy,
I just down loaded ME. This looks to be a great tool and I plan to show it at work. Thanks
I have been watching this thread and there are a few things I would like to add.
• When using double face tape, make sure everything is clean before applying the tape. Test to make sure that the coolant will not attack the tape.
• If a mister is left unused for a while it should cleaned before use. They can build up a mold and the next time it is used it will become air born.
• When it comes to cutting aluminum, stay away from any coatings that are gray to black. They are TiAlN (Titanium Aluminum Nitride), AlTiN (Aluminum Titanium Nitride), and TiAlSiN (Titanium Aluminum Silicon Nitride). Aluminum will stick and nasty thing will happen.
Another CAD/CAM package to check out is BobCad. They have sales every so often. We purchased 2 seats of mill and lathe for $1,500.

[sanddrag]

Originally Posted by Mr. Mike

Another CAD/CAM package to check out is BobCad. They have sales every so often. We purchased 2 seats of mill and lathe for $1,500.

I evaluated BobCAD/CAM (along with half a dozen others) and I can't say I'd recommend it based on my 2 hour demo of it. The UI and workflow seems primitive and complex compared to some other software packages. Also, once contact is initiated, be prepared to deal with their relentless sales force. You're basically on their contact list for life at that point, and you'll hear from them at least twice a month.

[roystur44]

Originally Posted by Mr. Mike

Roy,
I just down loaded ME. This looks to be a great tool and I plan to show it at work. Thanks.

It really is a great tool to have on your desktop. Simple and effective.

[James Tonthat]

Originally Posted by sanddrag

I evaluated BobCAD/CAM (along with half a dozen others) and I can't say I'd recommend it based on my 2 hour demo of it. The UI and workflow seems primitive and complex compared to some other software packages. Also, once contact is initiated, be prepared to deal with their relentless sales force. You're basically on their contact list for life at that point, and you'll hear from them at least twice a month.

We used HSMXpress last year for all our milling and worked for everything that we needed it for (pocketing, countersinks, bosses, contours, etc.). You provide your email address in exchange for their free version (HSMXpress, HSMWorks is their paid version). I think they emailed me once if I was interested in HSMWorks and haven't contacted me since. It's a pretty easy to use package with really good Solidworks integration. They were purchased by Autodesk a bit ago so they're working on an Inventor version.

One of the good parts of having a plug in program into your CAD program is when you do rev's they'll automatically rebuild into your CAM program so that all you need to do is re-post it for your G-code.


The 1/4" EM was definitely our workhorse last year and when we were newbs at it, we'd have it cut with the tip of the EM (broke a couple EM's). I later on predrilled a lot of the paths with a 1/4" drill then entered maybe 1" into the material using the top of the EM closer to the tool holder. It's all about balancing heat, your tools, your fixturing, and your machine. You'd be surprised how much you can push your tools with the HP/revs you have.

[DonRotolo]

Originally Posted by roystur44

I uploaded a machining calculator called ME consultant to the CD media section. It's a great simple freeware tool to find out basic speeds and feeds.

OK, so I finally downloaded ME Consultant, and I'm not sure that I'm understanding what I am seeing. The Help file doesn't open for me.

Referring to the image, can someone confirm for me that with the parameters shown (1/4" 4-flute HSS endmill cutting 6061 to a depth of about 1/8"), I should cut at about 72 IPM?

What do "Spindle %" and "Feed %" mean? I don't understand the percentage.

==============
On the topic of cooling, I went to Harbor Fright and bought an airbrush gun for $10. I ran the brush at about 20 PSI and it sprayed a nice fine mist of water (my test fluid), which I could vary from barely a mist to almost super-soaker level. The air action should blow away the chips from the cut, and the coolant will, um, cool it. I'm going to buy a gallon of Koolmist 77 from McMaster and see what it'll do with a scrap block of aluminum.

[Cory]

Originally Posted by DonRotolo

OK, so I finally downloaded ME Consultant, and I'm not sure that I'm understanding what I am seeing. The Help file doesn't open for me.

Referring to the image, can someone confirm for me that with the parameters shown (1/4" 4-flute HSS endmill cutting 6061 to a depth of about 1/8"), I should cut at about 72 IPM?

What do "Spindle %" and "Feed %" mean? I don't understand the percentage..

Those are reasonable numbers. I don't know what the % means, but I'm guessing you modified the spindle speed and left the chip load as they recommended it? It probably means that 10,000 RPM is 197% of the default speed it would recommend.

[roystur44]

Hi Don,

The manual is a standard windows help file. Try opening in another computer or I can print it out for you and send a pdf.

Snipped from the help manual


Spindle Efficiency is the percentage of the power produced by the machine spindle motor that's actually available to a cutting tool. For machines in good condition, this figure is normally in the 80% - 90% range.

When Feed % (feed override) is changed, feed outputs, machining times, material removal rate, and power requirements are recalculated.

The maximum value allowed for Feed % is 300.0

When the override is below 100.0, the Feed Reset button is blue. When exactly 100.0, the button is white. When above 100.0, the button is red.

[scottandme]

Originally Posted by Cory

Those are reasonable numbers. I don't know what the % means, but I'm guessing you modified the spindle speed and left the chip load as they recommended it? It probably means that 10,000 RPM is 197% of the default speed it would recommend.

Yup, I normally see around 300-400 SFPM as the suggested range for HSS end mills in 6061. In their database they're using 334 SFPM as the 100% (recommended) speed, and you're at roughly double that if you're running 10k RPM.

It's easy enough to look up the recommended numbers from your end mill manufacturer - here's Niagara http://www.niagaracutter.com/techinfo/index.html

As previously mentioned, I wouldn't suggest trying to slot with a 4-flute cutter in aluminum, especially with just mist. Any problems with chip evacuation (caused worse by increased heat - higher SFPM range) and the cutter is going to load up with aluminum and snap.

Carbide and fewer flutes (1 flute onsrud) solves those issues. At the very least you should reduce the depth of cut a bit so that the chips are smaller and can get out of the slot easier. Probably still have to babysit it and blow chips out of the slot manually.

[DonRotolo]

Originally Posted by scottandme

As previously mentioned, I wouldn't suggest trying to slot with a 4-flute cutter in aluminum, especially with just mist.

Agreed. Doing just a little online research yielded This Page, which (although quite long) helped me understand the issues I am facing. Boy oh boy, this is different from my ancient manual machines! But now I feel prepared to start experimenting in aluminum. With some 'used' end mills, so when they break I won't feel so badly.

[techhelpbb]

Originally Posted by sanddrag

I evaluated BobCAD/CAM (along with half a dozen others) and I can't say I'd recommend it based on my 2 hour demo of it. The UI and workflow seems primitive and complex compared to some other software packages. Also, once contact is initiated, be prepared to deal with their relentless sales force. You're basically on their contact list for life at that point, and you'll hear from them at least twice a month.

BobCAD is extremely aggressive about sales.
A bit too aggressive at times.

I find there interface a bit old fashioned in visual style but I have found that depending on your perspective of the CAD/CAM/CNC workflow BobCAD can be great product. I own a few versions with and without dongles.

There is unfortunately a learning curve.
I had the same trouble the first time I used it.
Once I got the hang of it things went smoother.
I could never have made due with a 2 hour demo either.

Originally Posted by Mr. Mike

• When it comes to cutting aluminum, stay away from any coatings that are gray to black. They are TiAlN (Titanium Aluminum Nitride), AlTiN (Aluminum Titanium Nitride), and TiAlSiN (Titanium Aluminum Silicon Nitride). Aluminum will stick and nasty thing will happen.

Does this not depend on the speed of the spindle?

Usually you have to spin the TiAlN end mills at higher speeds to make the coating operate as intended (18k to 22k RPM).
You would not want to use a TiAlN end mill too slowly or it will be worse than an HSS end mill.

Then there's the other issue, the higher the spindle speed the higher the IPM you need to move or risk rubbing. Not a problem for good machines but a problem for light weight gantry mills.


Generally and not in reply to anyone:
I linked this in a topic in the motor section but I will link it here as well:
http://blog.cnccookbook.com/2012/03/...tting-success/
Props to scottandme for posting a reference to G-Wizard as well (last page).

The issue I have with this topic is that I suspect that the different teams have different CNC machines.
A servo driven bridge or turret mill will have different requirements than a stepper driven gantry mill.
The bridge or turret has greater rigidity.
Depending on the spindle operating range it will impact the IPM.

It is hard to pick out what machine is what.
Some of the machines might be using steppers and therefore must target lower IPM feeds.
Some of the machines might have less cooling.
Some of the machines might have higher speed spindles with no ability to go slower.
The key elements that make this work depend on the knowing the machine sore spots.

For example:

Originally Posted by sanddrag

On our router at ~20,000 RPM, we've had a lot of trouble cutting aluminum with a standard 1/4" 3 flute carbide variable helix endmill we use with great results at 6,000 RPM with coolant on the mill. On the router, it just wants to load up and melt/weld chips. I'm thinking a 2-flute would give better chip evacuation.

Currently, our coolant system on the router is a student and a spray bottle of WD40.

I assume the mill in question is a turret type like a Bridgeport?

At this link...
http://www.daycounter.com/Calculator...lculator.phtml

Plug in 0.25", 300SFM, 3 flutes.
You get: about 4,500 RPM, 27.5 IPM
Makes sense that this works.

Plug in 0.25", 1,310SFM, 3 flutes
You get: about 20kRPM, about 120 IPM
This is probably not going to work.
I would be a bit suspicious of a carbide end mill rated at 1,310SFM uncoated.
Even more suspicious if your router can sustain the feed rate to keep it from rubbing.

At a spindle speed of 20kRPM I think you should consider a TiAlN end mill for the router with 2 flutes and 1/8" diameter.
That would get you:
655SFM, 20kRPM spindle speed, 80IPM feed.
If your gantry mill is outfitted with either really powerful steppers or servos it will work.

Try this:
http://www.wttool.com/index/page/cat...lls+%28USA%29/

Otherwise if you can't get the power from the steppers on your gantry:
Use a single flute as others have suggested and you'll divide that feed rate in half.
At that point if it's not enough edit your depth of cut and tool path to accommodate.

[scottandme]

Originally Posted by techhelpbb

Does this not depend on the speed of the spindle?

Usually you have to spin the TiAlN end mills at higher speeds to make the coating operate as intended (18k to 22k RPM).
You would not want to use a TiAlN end mill too slowly or it will be worse than an HSS end mill.

Anything with Al in the coating will not work to cut aluminum. Mainly for chromoly steels, stainless, titanium, nickel alloys, etc. They need high temperatures to "activate", which requires high SFPM numbers. From what I understand it actually creates a thin film of aluminum oxide when it hits that activation temperature. That's purely dependent on the size of the cutter and the material - but 18 to 22k is pretty extreme for a VMC - that's a specialized machine. Most are in the 8k to 12k range give or take. Generally with those cutters they don't use coolant (same with many carbide/ceramic insert cutters), just a heavy air blast to clear chips. The coolant can cause the insert to fracture from thermal shock.

For aluminum you either want uncoated, ZrN, or TiB2. TiCN can work well, but avoid TiN. Most major brands make geometry specifically for cutting aluminum (higher helix, polished flutes, etc, etc).

[techhelpbb]

Originally Posted by scottandme

Anything with Al in the coating will not work to cut aluminum. Mainly for chromoly steels, stainless, titanium, nickel alloys, etc. They need high temperatures to "activate", which requires high SFPM numbers. From what I understand it actually creates a thin film of aluminum oxide when it hits that activation temperature. That's purely dependent on the size of the cutter and the material - but 18 to 22k is pretty extreme for a VMC - that's a specialized machine. Most are in the 8k to 12k range give or take. Generally with those cutters they don't use coolant (same with many carbide/ceramic insert cutters), just a heavy air blast to clear chips. The coolant can cause the insert to fracture from thermal shock.

For aluminum you either want uncoated, ZrN, or TiB2. TiCN can work well, but avoid TiN. Most major brands make geometry specifically for cutting aluminum (higher helix, polished flutes, etc, etc).

So you are basing this on the VMC (Vertical Milling Center) not being able to obtain those high spindle speeds in general?

What if they are using a standard shop router(19kRPM - 25kRPM) or a RotoZip (15k-30kRPM) for a spindle on a homemade gantry?

Course the price they pay is not just for the coating it's also that they will need a high feed rate.
A high feed rate most smaller steppers would have difficulty achieving.

I agree with you if you slow down the spindle and operate more in the range of 8k-12k TiAlN is the wrong coating to use.

Without knowing what sort of machines each team is trying to use it gets a bit more involved.

[BrendanB]

Originally Posted by sanddrag

I evaluated BobCAD/CAM (along with half a dozen others) and I can't say I'd recommend it based on my 2 hour demo of it. The UI and workflow seems primitive and complex compared to some other software packages. Also, once contact is initiated, be prepared to deal with their relentless sales force. You're basically on their contact list for life at that point, and you'll hear from them at least twice a month.

We use BobCAD/CAM at work. It was a program we picked up in the spring to potentially use for robotics and potentially replace our current software since the yearly license fees were getting crazy for two seats. We have a few licenses with the goal that one will be on a machine at the school so the students can design parts and make the g-code to cut out a lot of the time that was spent manufacturing parts by the small staff available to work on parts for us.

We hear from those guys once a week every Monday (going to be awaiting their call tomorrow morning!) and while yes it is annoying they give us great deals on new software as well as amazing discounts on software we purchase additional seats of so its annoying but really nice. Their training staff is also great! Met a few of them at Eastec this year and they were very friendly and informative!

As for the program itself it took me a while to get the software down since it was my first experience with a creating tool paths but I went through their DVD instruction videos and from there on a little practice makes perfect. If their is one thing I wish they did better it would be their pan/zoom/rotation. Oh well.

On the brighter side it has been very easy to use on various machines in our shop that run on differing controllers which has been a good plus!

For FRC purposes I would see if you can talk to company to get the software for free.

[Cory]

Originally Posted by techhelpbb

At this link...
http://www.daycounter.com/Calculator...lculator.phtml

Plug in 0.25", 300SFM, 3 flutes.
You get: about 4,500 RPM, 27.5 IPM
Makes sense that this works.

Plug in 0.25", 1,310SFM, 3 flutes
You get: about 20kRPM, about 120 IPM
This is probably not going to work.
I would be a bit suspicious of a carbide end mill rated at 1,310SFM uncoated.
Even more suspicious if your router can sustain the feed rate to keep it from rubbing.

At a spindle speed of 20kRPM I think you should consider a TiAlN end mill for the router with 2 flutes and 1/8" diameter.
That would get you:
655SFM, 20kRPM spindle speed, 80IPM feed.
If your gantry mill is outfitted with either really powerful steppers or servos it will work.

1300 SFM is perfectly reasonable for uncoated carbide. Most vendors will recommend 700-2000 SFM for a carbide end mill with aluminum specific geometry.

TiAlN, AlTiN, and TiN are always bad for aluminum. They have an affinity for aluminum which leads to galling, causing your end mill to load up and break.

While you are correct that TiAlN and AlTiN are designed to perform best at elevated temperature, you could never even get them to that elevated temperature in aluminum as you would have to run without coolant and you would be guaranteed to melt your chips and pack the flutes long before getting up to temp, completely disregarding the fact that these coatings are not advisable in aluminum due to their physical properties.