Cutting time for simple 11.25"x12" sign.

[wolfeman]

I have been trying like crazy to cut Hack of the week #125. It has the camping trailer on it. I have tried three times and something stupid always goes wrong. My main question is it seems that taking almost 16 hours to cut that is way to long. I have it set 3D rough cut to use 1/4 in end mill .125 deep, 35 ipm, 40% step over at 16000 rpm. Kept getting to much smoke so I dropped the depth to 0.1 and it was much better. 3D finish cut is 1/8"Ball mill, .06 deep, 30 imp, 8% step over at 16000 rpm. It just seems like a long time for a cheap 11.25" x 12" sign. I am using an X-carve early version and v-carve pro 9. Any thoughts (besides just calling me stupid) would be appreciated. I start out with .75 thick materiel and end up with only .3 thick materiel which does not leave much for engraving.

[Rcnewcomb]

1/4 in end mill .125 deep, 35 ipm, 40% step over at 16000 rpm. Kept getting too much smoke

The reason you are seeing smoke is that the bit is making fine power that gets pulled back into the cut and heats up. It also causes poor finish quality.

For a lighter duty CNC changing to a single flute bit like an Onsrud 48-007 may help quite a lot.

In the meantime you can try slowing the RPMs down on your router if that is an option.

[ger21]

On my DIY machine, I do 3D finish passes at 150-175ipm, which is 5-6x faster than you are running.
Even with an X Carve you should be able to increase the feedrate on your finish passes, as they aren't removing much material.

[scottp55]

You should NOT be getting smoke EVER!
Bit at end of cut should be near room temp if you're in the sweet spot.
That .25" bit may be cooked as carbide hates heat and will dull a cutter fast(dull/dirty cutters also create heat/smoke).
Not sure about your machine, but Feed sounds slow...RPM is good for the BallNose if Feeds tweaked.
Can you try at least 60IPM in All axis(Plunge should be fairly close to X,Y speeds for 3D).
Hopefully somebody with your machine will chime in.
scott

[wolfeman]

Thanks you for your response. I really appreciate it. I will try what has been suggested.

[Leo]

CHIPLOAD

Chipload is the #1 least understood and yet MOST important thing to know about.

CHIPLOAD - is the answer to WHY - am I getting what I am getting ---> in your case - smoke

Chipload means how far the cutter advances into the cut per flute, for each Revolution of the spindle.
Sooo a chipload of .001 means each flute removed .001 of material per each full revolution of the spindle.

https://www.guhdo.com/chipload-calculator

I used the above calculator - not my favorite, actually means nothing to me - it's just the first one I found, in a really quick search. There are thousands to pick from - they ALL are the same calculation.

This particular one says you should be between .009 to .013. With your numbers you are at .001 --- I am assuming you have a TWO flute end mill. If you have a 4 flute end mill you are at .0005. No matter what, based on a scientific calculation, not opinion, you are way way to low on chipload. There are three things you can adjust - 1) Number of flutes (don't use more than 2 or 3) 2) RPM & 3) feedrate.

Your machine will have capabilities based on how rigid the machine is, or how the work in held down.

To MY OPINION - you should try to achieve at least .003-.005 to start and go up from there.

My rule of thumb is - you want to make chips, not dust.

Fast RPM means friction, means heat, means burning IF the feed is too slow - that is what you have.

[Bill_L]

In the photo below which I'm cutting as I type, the model is 12" by 6". I used a 2 flute .25 BN to rough with exactly the same stepdown and stepover as you but at 3ips and 8400 rpm. Took about 16 minutes to complete and it left .04" of material to clear on the finish pass. The photo shows the finishing pass in progress. I've used a 3 flute .125 BN. Stepover is 9%. Feed is 3 ips in both X and Y and my spindle speed is 4800 RPM utilizing an offset climb cut strategy. These parameters produce nice chips and a pristine finish on the wood. I see a lot of people doing 3D at near max RPM and very slow feed speeds which 12 years of experience has showed me to be unnecessary. My finishing pass on this model just completed in 38 minutes. The type of machine and the operating system also come into play. I have a ShopBot PRS Alpha that handles 3D work very well.

While calculating chip load to get you "in the ball park" is a good start, testing is essential. I personally get in the ball park then refine feeds and speeds with the ear and chips. When your refinement/testing gets you dialed in you can hear it and see it in the chips produced. It's a smooth sweet sound, not screaming or groaning.

[Leo]

In the photo below which I'm cutting as I type, the model is 12" by 6". I used a 2 flute .25 BN to rough with exactly the same stepdown and stepover as you but at 3ips and 8400 rpm. Took about 16 minutes to complete and it left .04" of material to clear on the finish pass. The photo shows the finishing pass in progress. I've used a 3 flute .125 BN. Stepover is 9%. Feed is 3 ips in both X and Y and my spindle speed is 4800 RPM utilizing an offset climb cut strategy. These parameters produce nice chips and a pristine finish on the wood. I see a lot of people doing 3D at near max RPM and very slow feed speeds which 12 years of experience has showed me to be unnecessary. My finishing pass on this model just completed in 38 minutes. The type of machine and the operating system also come into play. I have a ShopBot PRS Alpha that handles 3D work very well.

While calculating chip load to get you "in the ball park" is a good start, testing is essential. I personally get in the ball park then refine feeds and speeds with the ear and chips. When your refinement/testing gets you dialed in you can hear it and see it in the chips produced. It's a smooth sweet sound, not screaming or groaning.

This is .009 chipload

[Beltramidave]

Bill,

What are you using for a spindle to be able to run at 4800rpm? Thanks

[Xxray]

If fine detail is not required, increase stepover to 14%, probably will be no visible difference and will reduce cut time considerably. Also jack up feed rate to max, will only go so fast anyhow with Z movements.
Still sounds crazy excessive for a 1/8 bit and relatively small project, post file if able or at least a screen shot of settings.

I suspect your bit is fried, and no amount of chipload sweet spot calculations will help a dead bit cut better.

[Mikehell]

35 IPM seems really really slow. That could be why it's smoking. I typically run a 2 flute 1/4" bit at 1 or 2 inches per SECOND (120 IPM)

[Mikehell]

CHIPLOAD

Chipload is the #1 least understood and yet MOST important thing to know about.

CHIPLOAD - is the answer to WHY - am I getting what I am getting ---> in your case - smoke

Chipload means how far the cutter advances into the cut per flute, for each Revolution of the spindle.
Sooo a chipload of .001 means each flute removed .001 of material per each full revolution of the spindle.

https://www.guhdo.com/chipload-calculator

I used the above calculator - not my favorite, actually means nothing to me - it's just the first one I found, in a really quick search. There are thousands to pick from - they ALL are the same calculation.

This particular one says you should be between .009 to .013. With your numbers you are at .001 --- I am assuming you have a TWO flute end mill. If you have a 4 flute end mill you are at .0005. No matter what, based on a scientific calculation, not opinion, you are way way to low on chipload. There are three things you can adjust - 1) Number of flutes (don't use more than 2 or 3) 2) RPM & 3) feedrate.

Your machine will have capabilities based on how rigid the machine is, or how the work in held down.

To MY OPINION - you should try to achieve at least .003-.005 to start and go up from there.

My rule of thumb is - you want to make chips, not dust.

Fast RPM means friction, means heat, means burning IF the feed is too slow - that is what you have.

This is one reason I like Onsrud bits. They actually publish the chip load for all their bits in the back of the catalog. If I get an elChepo bit I try to figure out which Onsrud it may be similar to and do the math from there

[Adrian]

The other thing to bear in mind is that with the nature of 3D toolpaths the feedrate you're actually achieving may be nowhere near what is programmed. That's because of the amount of Z movement.

Just something to be aware of when working out chiploads.

[Bill_L]

I have a Colombo spindle.

[LittleGreyMan]

Here's a video from Tools Today about chipload:

https://www.youtube.com/watch?v=fnu2uxVl80A

Nothing new under the sun, Leo and others already explained the concept, but you'll see machines cutting at the right feeds and speeds.