# Can I cut at 600 ipm? Video added!



## difalkner (Jan 3, 2012)

Yes, definitely!! Did I mean to do that? Absolutely *not*!!

I have made several changes to the toolpath profile for cutting the Longworth chucks and all for the better. When I started cutting them 100 chucks and almost a year ago the feed was 125 ipm, 18k rpm, 0.125" depth of cut, with a 1/4" downcut spiral bit. These chucks are 1/2" Baltic Birch and I knew this was conservative but I tend to stay on that side. I have slowly crept the speed up to where I am now cutting chucks at 250 ipm and all the other specs are the same except depth of cut is now 0.2".

When I opened the file for the 16" chuck I realized it was still at 200 ipm for the outer profile, with tabs, so I changed it to 250 ipm. Or so I thought... What I actually did was replace the '2' with '250' and didn't delete the extra '00'. My new feed rate was now 25000 but since I thought I had overwritten the 200 all I did was hit Ok and went out to the shop.

Everything cut just fine until it got to the outer profile. The ramp was at 250 ipm but when the cut reached the 0.2" depth it jumped up to 600 ipm, which is the max setting I have on the X & Y steppers. I was in a mild state of shock for a second trying to figure out what had happened but it cut around that 16" circumference so quickly that all I basically did was watch it cut. And it cut perfectly! The 3kW (4HP) spindle didn't blink at what I had inadvertently thrown at it, the bit was cool when it finished, and the edge was just as clean as it could be.

I don't plan to move any future cuts to 600 ipm but I have to say, now that it's over and nothing broke, it was fascinating watching it cut that fast! :grin: This Saturn frame is one stout and rigid CNC setup!

















I have a camera in the shop but the output is proprietary and requires its own player. If I can figure out how to export that to something I can upload to YouTube I'll show y'all.

David


----------



## UglySign (Nov 17, 2015)

Nice David! ... Triplify production?


----------



## OCEdesigns (Jan 31, 2019)

That had to be a little un-nerving as soon as it started moving!!


----------



## difalkner (Jan 3, 2012)

OCEdesigns said:


> That had to be a little un-nerving as soon as it started moving!!


You have no idea!! LOL! In the video I can see me whipping around to look at Mach4 to see what the speed was and it showed 600, which is about what it looked like when it was making the circle. 

Rapids are set at 600 ipm and I see that all the time but it's in a straight line and not cutting anything. 600 ipm _*cutting *_in a 16" circle is really fast!

David


----------



## rwl7532 (Sep 8, 2011)

Clean your glasses.


----------



## Danman1957 (Mar 14, 2009)

Wow


----------



## difalkner (Jan 3, 2012)

rwl7532 said:


> Clean your glasses.


The cleanest glasses in the world won't do any good at all if you never look at what you type. :wink:

New SOP - type, review, type, review, type, review, ad nauseum :grin:

David


----------



## 4DThinker (Feb 16, 2014)

A few years back I spent some time doing the math to calculate optimum feed speeds for certain bits with specific depth of cut and spindle speed. I kept getting numbers far faster than my Probotix hardware limits (200ipm). They implied I could cut through 3/4" hardwood in one pass with a 2-flute upcut bit and the chips produced would be carrying away the heat generated. Now the older Probotix CNCs would complain about such a cut, but our shop technician often does such cuts on the large Multicam industrial CNC we have. The routers we use would also complain if pushed too fast through hard wood even if the bit was keeping up with chip removal. The more face of a bit cutting wood the more drag there is against the router motor. 

You've given me something to try this weekend. I often cut tenons on the end of hardwood boards. I'll make some test scraps, then cut 3 (or more) versions of the same toolpath, with pass depth the only thing I change between tenon cutting tests. I suspect my meteor can handle all variants ( 1/4" pass, 1/2" pass, 3/4" pass) despite me normally 1/8" per pass with a 1/4" upcut spiral. There may be some difference in the finished face of the cuts. I'll report back. 

4D


----------



## RainMan 2.0 (May 6, 2014)

I didn’t realize or couldn’t visualize how fast it was going till I broke it down into seconds .
So your cutting 10” per second? 
Obviously not in one pass ,but in multiple passes at different depths .
I wonder if that’s hard on the machine itself?


----------



## ger21 (Feb 10, 2019)

On our machine at work, we normally cut 3/4" plywood and particle board at about 800-850/min with a 3/8" or 1/2" 2 flute bit. With a 3 flute, I've at at about 1250ipm. At these speeds, holding your parts can be a real issue.


My normal speed with a 1/4" bit is 400-450ipm.

The two main limitations with hobby machines are spindle power, and machine rigidity. 1/4" bits don't take a lot of power, so it comes down to whether or not the machine flexes.


----------



## RainMan 2.0 (May 6, 2014)

ger21 said:


> On our machine at work, we normally cut 3/4" plywood and particle board at about 800-850/min with a 3/8" or 1/2" 2 flute bit. With a 3 flute, I've at at about 1250ipm. At these speeds, holding your parts can be a real issue.
> 
> 
> My normal speed with a 1/4" bit is 400-450ipm.
> ...


I never considered that the speed would put more pressure on the part your cutting .
Good to keep in mind


----------



## 4DThinker (Feb 16, 2014)

Results are in with my quick tenon test. The Meteor didn't balk at any of the 2 toolpaths I've done. Wood was white oak, scraps from a pallet I took apart. End grain cuts. 

First test: 1/4" deep passes, 1/8" stepover, 3/4 total depth. Climb cut perimeter profiles. The feed speed self limited as it went around the perimeter, slowing down on the curves, speeding up most on the long straight side. Despite being set at 200ipm the speed never got higher than 60ipm on the straights. Finished surface looks fine and tenon measures within .002" of what I'd programmed it to be. 

Second test: 1/2" deep passes, 1/8" stepover. 1" total depth. Feed speed same as above. Finished surface looks/feels a little rougher than before. Tenon measures larger than programmed, implying the climb cut deflected somewhat as it went around the tenon. I suspect a followup conventional pass would clean up the surface and bring it down to the final dimension. 

I do a climb cut with a 1/4" spiral upcut bit as it leaves the shoulder of the tenon cleanly cut. A conventional profile pass typically splinters out the edge. 

Chip were larger than when I do a 1/8" pass, and threw considerable farther (3x farther) from the router. Dewalt 2.5hp router set at 5 (of 6 max) speed. 

I've concluded I can do similar tenons using a 3/8" pass depth, or 2 passes max on anything up to 3/4" depth. Face grain cuts using the whole width of a bit I'll keep at 1/8" or 3/16" pass depth, depending on the wood I'm cutting. 

This points out that if one always only cuts 1/8" deep at a time, only the last 1/8" of a bit is being used and it will get dull 3x as fast as it has to do 6 passes while a 1/4" pass depth would only need to do 3 passes for a 3/4" deep cut. The job will finish in 1/2 the time. Aspire has a last pass offset option that can let you do the final face of a cut as if done in one pass with the bit. 

4D


----------



## difalkner (Jan 3, 2012)

RainMan 2.0 said:


> I didn’t realize or couldn’t visualize how fast it was going till I broke it down into seconds .
> So your cutting 10” per second?
> Obviously not in one pass ,but in multiple passes at different depths .
> I wonder if that’s hard on the machine itself?


No idea, Rick. The Saturn didn't seem to mind at all but it sure gave me the heebie jeebies! :grin:



ger21 said:


> On our machine at work, we normally cut 3/4" plywood and particle board at about 800-850/min with a 3/8" or 1/2" 2 flute bit. With a 3 flute, I've at at about 1250ipm. At these speeds, holding your parts can be a real issue.
> 
> My normal speed with a 1/4" bit is 400-450ipm.
> 
> The two main limitations with hobby machines are spindle power, and machine rigidity. 1/4" bits don't take a lot of power, so it comes down to whether or not the machine flexes.


A friend owns a cabinet shop about 10 minutes from our house and he bought a new $100k CNC last year to replace his worn out machine. I watched it cutting 3/4" plywood like you mentioned. I don't recall the feed rate but it was far faster than my measly 600 ipm, seems like he said it was up around 1000 ipm but I don't know what bit he was using.

I think the Saturn is rigid enough and the spindle powerful enough to go much faster than the 250 ipm I have been cutting at but for what I normally cut, which is typically smaller items except for the larger Longworth chucks, 250 ipm just feels about right. Of course, when I first started on the CNC 125 ipm felt about right.

Do you have any video of your machine cutting at 400-450 ipm, Gerry? I'd love to see that.

David


----------



## difalkner (Jan 3, 2012)

4DThinker said:


> End grain cuts.
> 4D


Good test! I have found end grain really sweet to cut, a lot different than face or edge grain.

David


----------



## ger21 (Feb 10, 2019)

difalkner said:


> Do you have any video of your machine cutting at 400-450 ipm, Gerry? I'd love to see that.
> 
> David



No, and you can't really see anything.
Here's basically the same machine, probably cutting in the 800ipm range. Cutting starts at the 1:00 min mark. The beginning is drilling with the drilling head.


----------



## difalkner (Jan 3, 2012)

It just doesn't look that fast on a big machine like that. 600 ipm on our little 2x4 machine seems very fast!

Is the gantry cantilevered on that machine? Seems like that would not be ideal, like it may have some flex out on the end of the gantry. I realize it's probably very strong, but still...

David


----------



## ger21 (Feb 10, 2019)

Yes, it's cantilevered, and about 6 ft long. It's a roughly 16"X6" square tube, 1/4" steel. It probably has at least 1000lbs hanging on it too.

There's actually almost zero flex under most conditions. It has S-Curve acceleration, which makes it start and stop very smoothly, with no jerkiness. And it accleerates very fast. It'll get to 800ipm in about 2 inches.

Their new machines are not cantilevered, but it is really nice at times. Much easier to load 12ft sheets from the side, rather than the end.


----------



## difalkner (Jan 3, 2012)

*Video added*

Ok, here's the video of my little 'incident' on the CNC, cutting at 600 ipm - 






David


----------



## BalloonEngineer (Mar 27, 2009)

Don’t want to make you scared any more, but since you told it to feed 25000ipm, Mach4 obediently allowed X-axis and Y-axis to EACH go to their max of 600ipm and at all but 4 points (North, East, South and West) it was going faster than 600, up to 845 or so.


----------



## MEBCWD (Jan 14, 2012)

David maybe you standing right there when your CNC started the 600IPM makes it look faster than the other machine running at 800IPM. The "in your face moment" when something like this happens.

If mine did that it would the "on the floor moment" when the CNC came apart.


----------



## RainMan 2.0 (May 6, 2014)

Watching the video I don’t think your Saturn was breaking sweat . Nice looking setup you have their David


----------



## ger21 (Feb 10, 2019)

I once had a typo, and tried to cut at 1200ipm and 1500rpm. It got about an inch before the 1/2" carbide bit snapped.


----------



## difalkner (Jan 3, 2012)

Wow! Snapping a 1/2" bit takes some serious force, I would imagine. Btw, I can testify that breaking a 1/8" bit is like breaking a toothpick. :grin:

David


----------



## ger21 (Feb 10, 2019)

Yes, industrial machines can easily kill you if you get in there way. :surprise:


----------



## UglySign (Nov 17, 2015)

Lol... toothpick

I can testify that a 1/16" bit does snap upon touching when
you set it for one pass in 1/8" AL. Supposed to go only in small
increments to clear some areas that a 1/8"bit couldnt get to.
Of course I only had one bit. I find when some days seem
good to go, troubles waiting.


----------



## 4DThinker (Feb 16, 2014)

It might be worth clocking how long it took to cut around the large perimeter as you know the diameter and can calculate the circumference. That would let you know how fast it really cut. I say this as with curves my CNCs including the big industrial multicam the acceleration and deceleration between nodes usually self-limits the top speed to something under the machine's max hardware limit. If you get a number less than 600, and your cut finished with no damage to the bit or project, you will have a good idea just how much faster you can push all your future CNC jobs. I get around 430ipm doing a quick calc starting and stopping your video. 50.26" circumference in about 7 seconds to make one perimeter pass. You could probably bump your 250 up to 400ipm with no detrimental effects. 

4D


----------



## difalkner (Jan 3, 2012)

4DThinker said:


> I get around 430ipm doing a quick calc starting and stopping your video. 50.26" circumference in about 7 seconds to make one perimeter pass. You could probably bump your 250 up to 400ipm with no detrimental effects.
> 
> 4D


I timed it 3 times and got 5.24, 5.24, and 5.26 so just using 5.25 seconds gives me about 575 ipm. Using my video editing software I can set a mark where the 600 ipm starts and completes one full circle and it shows 5.03 seconds. If I use that data then that calculates to 599.5 or just simply 600 ipm, which is the max setting for the steppers.

We just got another order for a 12" Longworth chuck that I'll cut tomorrow morning and I think I will leave the slots at 250 ipm but bump the outer perimeter to 350 ipm to see how that does. 

I also realize my depth of cut of 0.2" is conservative and I have a few of these 1/4" downcut spiral bits that are sharp enough to use but don't give as clean a cut as a brand new bit. The bit I'm using now is still pretty sharp but I'm thinking of using one of the older bits that has basically only cut 0.2" and setting a new depth of cut of 0.25" to introduce a sharp cutting edge for that last 0.050" and see how that does. Does that make sense and does it seem like a good thing to try out?

David


----------



## beltramidave (Jan 6, 2016)

For what it's worth, this is what GWizard Calc comes up with.


----------



## difalkner (Jan 3, 2012)

So at 18k rpm and 300 ipm I'd be about the same as that shows. I may give that a shot. Thanks, Dave!

David


----------



## 4DThinker (Feb 16, 2014)

This is unrelated to max feed speed, but I've just done another tenon test using some red oak scraps. 1/4" spiral upcut end mill. This time 2 profile climb passes 3/4" deep, 1/16" stepover, followed by a conventional profile pass stepping over .002" to skim off any width missed by by possible deflection during the previous pass. The tenon end up with smooth faces, and exactly the same width and thickness as programmed. Bit was cool to the touch. Chips were 3/4" long, no "dust" I could see wafting up during the cut. The larger chips flew out nicely and being larger dropped quickly to bed and surrounding floor. 

I did a second test, a single profile climb pass 3/4" deep, 1/8" stepover, followed by a conventional profile pass stepping over .002" to clean up. The feed speed was 1/2" what I used in the first test. I noticed during the first test feed speed maxed out at about 60ipm going around the tenon, so I kept the second pass at 30ipm. Again, the tenon faces were smooth and exactly as wide and thick as programmed. Both tests used a 1/2" long 45 degree lead-in so the bit wouldn't plunge vertically into the wood. 

These tests are mainly because I realized that my normal default pass depth for any bit is 1/2 the bit diameter. This results in max moment load on the bit as it goes forward, all wear on just the ends of the bits. By making profile passes using all or most of the bit's available cutting height the whole blade will wear evenly. A perimeter cutout can finish in 1/6 the time (six 1/8" passes vs one 3/4" pass) and even if I cut feed speed in half the job can finish in 1/3 the time. My meteor CNC didn't complain during the cuts. 

This is just for outside profile passes using half or less than half the width of the bit. For through cuts using the whole width of the bit I'll stick to 1/2 the bit width per pass. For pocket cuts with an initial full width cut followed by stepover cuts to clear the pocket, I'll double the pass depth but manually slow down the initial pass and ramp into the wood rather than plunge straight in. In fact I may try a ramp in to full depth of a pocket, manually slowed, and setting the stepover to 15%-25% of the bit width for clearing out the rest of the pocket. Again the advantage is in using the whole cutting height of the bit when I can. 

4D


----------



## difalkner (Jan 3, 2012)

Do you have video of these tests? That would be most helpful.

David


----------



## 4DThinker (Feb 16, 2014)

I did shoot video of the initial tests using white oak, but not the latest red oak tests. I'm hesitant to upload those video clips as they are 4K and my service provider caps upload speeds to a crawl. If I do get around to uploading the videos they''ll be on my blog rather than on YouTube. 

4D


----------



## difalkner (Jan 3, 2012)

Or you can convert them for YouTube and put the 4k version on your blog. Let us know if/when you put them, please sir.

David


----------



## 4DThinker (Feb 16, 2014)

If it helps any, here are photos I took of the white oak test results and the mess they made. 4D


----------



## difalkner (Jan 3, 2012)

Yeah, it makes a mess but I sure like cutting end grain. It cuts like butter!

David


----------



## 4DThinker (Feb 16, 2014)

Since you mentioned butter, I suspect somewhere out there should be evidence of a CNC actually cutting frozen butter. I'm gonna guess cutting end grain is still more fun.


----------



## SteveMI (May 29, 2011)

I have a related story. For couple years I had access to two ShopBot tables, with the square 5 hp spindles. Using a Vortex 3/8" compression bit I could cut 3/4" baltic birch at 400 ipm in one pass. I think it could have cut faster, but the shop wanted the 400 ipm max. That access went away and I can now use a ShopBot with the 2.2 kw round spindle found all over ebay. So, I figured to repeat my experience. It plunged and went about 8 inches before stalling the servos. It took me about a minute to figure out the difference - horsepower. No more single pass, resorted to two passes and it works at 400 ipm. BTW - mainly doing it making knock offs of the Festool MFT tables, 20 mm holes on 4" centers. 
Steve.


----------



## difalkner (Jan 3, 2012)

As in racing, horsepower means everything! Good story, Steve. I have a rigid machine and 4HP and am reluctant to cut 1/2" BB in one pass. I'm thinking of getting this Whiteside 1/4" compression bit and using two passes for the Longworth chucks.

David


----------



## SteveMI (May 29, 2011)

difalkner said:


> As in racing, horsepower means everything! Good story, Steve. I have a rigid machine and 4HP and am reluctant to cut 1/2" BB in one pass. I'm thinking of getting this Whiteside 1/4" compression bit and using two passes for the Longworth chucks.
> 
> David


I use a Whiteside UD4122 3/8" compression with good results on solid wood, primarily waste area passes with Fusion. Chipload is spec'd at 0.016 to 0.022. GWizard tells me 100 ipm full 3/8" cutting at 8,000 rpm. The Vortex is my go to for ply.
Steve.


----------



## difalkner (Jan 3, 2012)

I cut the slots on the Longworth chuck at 0.26" so using a 1/4" bit is necessary. Looks like it's time for me to consider additional tooling to cut these. 

David


----------



## Scottart (Jan 8, 2015)

fascinating Dave, and thanks for posting the video and a glimpse of you and your shop set up...


----------



## difalkner (Jan 3, 2012)

Scottart said:


> fascinating Dave, and thanks for posting the video and a glimpse of you and your shop set up...


Glad I had that video, Scott, but wish I had audio with it. Btw, there are plenty of shots of the shop in the videos on my YouTube channel if you haven't checked it out.

David


----------

