[wtopace]

Hey guys, first post on cnczone for me. I recently got a Tormach PCNC1100 and it is my first CNC machine. I have been running manual lathes and mills for 4-5 years, but CNC is very different... in a good way! I have been working with CAD software since high school, so that part is already pretty natural to me. I have been using Sprutcam that I ordered with the mill and so far it seems pretty straight forward.

On to the problem... I am trying to drill quite a few 1/16" holes 1/2" deep. Speeds and feeds were determined with GWizard and peck depth was determined from reading a considerable number of threads with "working" formulas. I originally settled on 200% diameter as peck depth, but the bit broke on the 5th hole, this was a precision twist cobalt bit. I ordered a pack of 12 Irwin (China) cobalt bits from Amazon and decided to do a little stress test. Note: The first Irwin bit had considerable runout at 300rpm in the chuck so I removed it and the 2nd bit was much better. I am not sure what the procedure is to "indicate a drill bit" as I have read online, however, I am always happy to learn.

The test is as follows:

Material: 6061 Aluminum
RPM: 5100 (GWizard)
Feed rate: 2.947 (GWizard)

Row1: 50% diameter peck depth
Row2: 100% diameter peck depth
Row3: 150% diameter peck depth
Row4: 200% diameter peck depth

Unfortunately, the bit didn't even make it past the first row, it broke on hole 6 out of 10.

https://www.youtube.com/watch?v=gtyRjIZ1F0U

Any help or suggestions would be greatly appreciated!

[alan_3301]

I would run max rpm around 10k rpm on that machine?
I am getting 11.4k rpms and 4 ipm with gwizard.

s

[wtopace]

The PCNC1100 maxes out at 5100, I believe the smaller PCNC770 has a 10k spindle.

[rcs60]

I would try a parabolic drill like Guhring Mfr Part #: 9005490015900 which can be purchased from MSC #: 85758043 $6.04 ea. it is a high speed drill bright finish coating which allows the aluminum to flow out the drill flutes better some of the parabolic drills can be run at 10x drill depth which would eliminate or reduce the pecking cycles as for spindle speed probably as fast as the spindle would go and .0005 per flute for a feed rate

rcs60

[WOTDesigns]

First I would share that you are spot drilling along with the feeds and speeds (good job listing those by the way). I know it is in the video, but its a lot easier and faster to read than watch a video.

200% peck cycle on a drill that small is ballsy and only likely to work out if you were able to reach the appropriate speeds for the material which you aren't even close; at 5Krpm you are barely half of the correct spindle speed. You can easily get a first and maybe second peck at that but after you should be at 50-100% diameter at the ABSOLUTE MAX.

You are far too slow on the feed for drilling. Just because it is little doesn't mean you should baby it. You are creeping into the material which is packing long chips into the flutes and since you are moving so slow they are getting hot and likely causing your problem. Decrease your peck to 50% diameter and double (or more) your IPM and you will be fine. MOVE FAST when in the hole. Make a chip big enough to carry heat away from the hole. Drill bits LIKE being pushed on and HATE sitting in a hole spinning and 5K RPM and rubbing the sides of the hole.

If you are doing these for production I can help you create a quick macro to take the first peck at 200% second at 100% and the rest at 50% and I would bet my lunch you will drill 1000 holes without changing a bit. I drill thousands of holes with #50 drill for 2-56 (roll form) and I only change the bit after every 4,000 holes because that is how many are in a production run. I will grab the actual speeds and feeds from that program in a few minutes, but you will find is a LOT faster.


EDIT: Actual peck cycle. Note the initial peck is nice and deep and I am moving at 9 IPM.

G20 
G00 G17 G40 G49 G80 G90 
( NO. 50 DRILL - WOT | TOOL - 3 | DIA. OFF. - 3 | LEN. - 3 | TOOL DIA. - .07 ) 

G52 X0 Y0 
M06 T3 
G43 H03 

G00 G90 
S5140 M03 (DRILL) 

[......]

N1001 (DRILL SEQUENCE) 
G00 Y0 
G90 
G01 Z0.1 F50. 
G01 Z-0.2 F9. 
G00 Z0.1 
Z-0.19 

G01 Z-0.28 
G00 Z0.1 
Z-0.27 

G01 Z-0.32 
G00 Z0.5 
M99

[wtopace]

I would try a parabolic drill like Guhring Mfr Part #: 9005490015900 which can be purchased from MSC #: 85758043 $6.04 ea. it is a high speed drill bright finish coating which allows the aluminum to flow out the drill flutes better some of the parabolic drills can be run at 10x drill depth which would eliminate or reduce the pecking cycles as for spindle speed probably as fast as the spindle would go and .0005 per flute for a feed rate

rcs60

Thanks for the suggestion, if I can't get standard drills to work then I'll definitely go this route. I have heard nothing but great things about the Guhring parabolic drills.

First I would share that you are spot drilling along with the feeds and speeds (good job listing those by the way). I know it is in the video, but its a lot easier and faster to read than watch a video.

200% peck cycle on a drill that small is ballsy and only likely to work out if you were able to reach the appropriate speeds for the material which you aren't even close; at 5Krpm you are barely half of the correct spindle speed. You can easily get a first and maybe second peck at that but after you should be at 50-100% diameter at the ABSOLUTE MAX.

You are far too slow on the feed for drilling. Just because it is little doesn't mean you should baby it. You are creeping into the material which is packing long chips into the flutes and since you are moving so slow they are getting hot and likely causing your problem. Decrease your peck to 50% diameter and double (or more) your IPM and you will be fine. MOVE FAST when in the hole. Make a chip big enough to carry heat away from the hole. Drill bits LIKE being pushed on and HATE sitting in a hole spinning and 5K RPM and rubbing the sides of the hole.

If you are doing these for production I can help you create a quick macro to take the first peck at 200% second at 100% and the rest at 50% and I would bet my lunch you will drill 1000 holes without changing a bit. I drill thousands of holes with #50 drill for 2-56 (roll form) and I only change the bit after every 4,000 holes because that is how many are in a production run. I will grab the actual speeds and feeds from that program in a few minutes, but you will find is a LOT faster.

Thanks for the great reply. I am still learning what real milling and drill should sound like. I'm afraid that I have spent the past few years on my manual just babying everything, I will learn in time though.

I'll standby and wait for your speeds and feeds suggestions and I'll give it a try and report back.

[WOTDesigns]

Any time. Odds are you only thought u were babying it on the manual. The chips I pull off my drill press are many times thicker than I get off my CNC.

BTW I only use HSS drill bits. They are SHARP and last long enough (thousands of holes of a $5 bit) but for production I use parabolic if available.

Brian
WOT Designs

[AUSTINMACHINING]

I use Kool mist for hsm cutting, but it sucks for drilling. Wd 40 works great. Deep holes are hard to cool so lubrication to reduce friction is key imo.

[wtopace]

I'm using the coolant that Tormach sells, it seems to be working decently so far, at least it keeps the rust at bay and with a few mods blows the chips away great.

I gave it another go with the following and broke the drill on the 6th hole.

RPM: 5100
Feed: 7 ipm
Peck depths: 0.156, 0.081, 0.031, 0.031... to 0.5" deep (this is 250% diameter for first peck or 0.156, decremented by .075 with a minimum of 50% diameter or 0.0313)

Perhaps these standard twist drills weren't designed to drill 8 diameters deep and I am just past the envelope of the cutter? It looks like your example above is cutting about 4.5 diameters deep.

Another boring video for anyone who is super bored.
https://www.youtube.com/watch?v=6dnjaoFFuM8

[bhurts]

Try putting that drill into a collet instead of a Chuck.

Ben

[zamazz]

You're problem could very well be the brand of drill. I've used Irwin taps from Home Depot before (only thing I could get on a Sunday) and they were garbage. One or two holes and they would snap, whereas an Emuge or OSG would last hundreds. Most of these cheap brands are meant for one time diy use, not for machine tools. I typically stay away from Chinese cutting tools. There are far better areas to save money and frustration on. We use mostly Nachi drills, but you can't go wrong with a US made split point drill.

A week ago I ran a job on our Tormach drilling a .067 hole 1.25 deep in 6061. It was so deep I was past the flutes into the shank of the drill, which I wouldn't recommend but it worked. I used a Nachi drill at 5100 rpm and used a .030 peck depth with full chip removing. I don't remember the exact feed rate, but I think it was a bit slower than 5. It worked perfectly for all 70 holes, so what your trying to do is certainly possible.

[WOTDesigns]

Zamazz is right on brand. Irwin is cheap compared to its cost. My local tool supplier carries Precision Twist Drill (PTD) which are American and good for everything I've ever needed, but they can also be had from KBC TOOLS for 20% less when my local KBC has what I need in stock (which is on my way to my normal tool supplier)

Brian
WOT Designs

[wtopace]

I definitely understand about the China cutting tools, hence the reason I specified it in my original post. Unfortunately, it was all I had available at the time.

I think I am going to re-engineer the design to use 1/8" offset holes instead of 1/16" on-center holes and see how it goes. What do you think of the following:

Drill: 1/8" HSS
RPM: 5100
Feed: 12 IPM
Peck depths: 0.250, 0.125, 0.0628, 0.0625 (If this becomes a production part, I can revisit these numbers to make them more aggressive and drill in 3 passes, but for now this is just a prototype)

Thanks again for all of the replies, this has been very helpful.

[WOTDesigns]

Should be a breeze

Brian
WOT Designs

[Steve Seebold]

Hey guys, first post on cnczone for me. I recently got a Tormach PCNC1100 and it is my first CNC machine. I have been running manual lathes and mills for 4-5 years, but CNC is very different... in a good way! I have been working with CAD software since high school, so that part is already pretty natural to me. I have been using Sprutcam that I ordered with the mill and so far it seems pretty straight forward.

On to the problem... I am trying to drill quite a few 1/16" holes 1/2" deep. Speeds and feeds were determined with GWizard and peck depth was determined from reading a considerable number of threads with "working" formulas. I originally settled on 200% diameter as peck depth, but the bit broke on the 5th hole, this was a precision twist cobalt bit. I ordered a pack of 12 Irwin (China) cobalt bits from Amazon and decided to do a little stress test. Note: The first Irwin bit had considerable runout at 300rpm in the chuck so I removed it and the 2nd bit was much better. I am not sure what the procedure is to "indicate a drill bit" as I have read online, however, I am always happy to learn.

The test is as follows:

Material: 6061 Aluminum
RPM: 5100 (GWizard)
Feed rate: 2.947 (GWizard)

Row1: 50% diameter peck depth
Row2: 100% diameter peck depth
Row3: 150% diameter peck depth
Row4: 200% diameter peck depth

Unfortunately, the bit didn't even make it past the first row, it broke on hole 6 out of 10.

https://www.youtube.com/watch?v=gtyRjIZ1F0U

Any help or suggestions would be greatly appreciated!

Your first mistake is using cobalt drills in aluminum. The web on a cobalt drill is WAY too thick to be drilling aluminum. The thick web of a cobalt drill doesn't allow enough chip clearance to get the chips out of the hole.

Second mistake is using Chinese drills. If I had to use only Chinese tooling, I would get out of machining. I don't use anything but Guhring drills. They're made in Germany, and yes they are on the expensive side, but they work.

I gave a job on my machine right now that I have to drill a .078 diameter hole 4 inches deep in 3/16 thick 6061 aluminum. I have run this job several times in the past, and I have NEVER broken a drill in that hole.

When I drill a hole like that, I will use a ball nosed end mill and 2 drills. I will use the end mill as my center drill and drill about .180 deep, then I will use a stub drill and drill that hole .500 to .750 deep, then I will put the long drill in and drill the rest of the way.

It takes about 6 minutes to drill that part, but I have never had a drill break in the part, or break out the side of the part.

[bill south]

I don't know if this has been mentioned earlier since I didn't read all the above but have you put a dial indicator and reference pin in the chuck and tested it for runout? A drill that small will snap with just a bit of side loading.
Good luck.
Bill

[popspipes]

I use Kool mist for hsm cutting, but it sucks for drilling. Wd 40 works great. Deep holes are hard to cool so lubrication to reduce friction is key imo.

+1 on the wd40, also kerosene or tranny fluid, Relton A-9 works well for drilling deep holes.

All the coolants I have tried are ok for cutting but not so good for drilling deep holes in aluminum.

[popspipes]

Hey guys, first post on cnczone for me. I recently got a Tormach PCNC1100 and it is my first CNC machine. I have been running manual lathes and mills for 4-5 years, but CNC is very different... in a good way! I have been working with CAD software since high school, so that part is already pretty natural to me. I have been using Sprutcam that I ordered with the mill and so far it seems pretty straight forward.

On to the problem... I am trying to drill quite a few 1/16" holes 1/2" deep. Speeds and feeds were determined with GWizard and peck depth was determined from reading a considerable number of threads with "working" formulas. I originally settled on 200% diameter as peck depth, but the bit broke on the 5th hole, this was a precision twist cobalt bit. I ordered a pack of 12 Irwin (China) cobalt bits from Amazon and decided to do a little stress test. Note: The first Irwin bit had considerable runout at 300rpm in the chuck so I removed it and the 2nd bit was much better. I am not sure what the procedure is to "indicate a drill bit" as I have read online, however, I am always happy to learn.

The test is as follows:

Material: 6061 Aluminum
RPM: 5100 (GWizard)
Feed rate: 2.947 (GWizard)

Row1: 50% diameter peck depth
Row2: 100% diameter peck depth
Row3: 150% diameter peck depth
Row4: 200% diameter peck depth

Unfortunately, the bit didn't even make it past the first row, it broke on hole 6 out of 10.

https://www.youtube.com/watch?v=gtyRjIZ1F0U

Any help or suggestions would be greatly appreciated!

I notice in your video that the spindle nose appears to have a black plastic or rubber boot on it? I wonder if thats something on the new machines?

[WOTDesigns]

Not sure why I didn't notice when I watched the video the first time but you are also using a drill chuck which tend to have more run out then ER chucks.

I always use ER chucks for small drill bits.

Brian
WOT Designs

[wtopace]

I notice in your video that the spindle nose appears to have a black plastic or rubber boot on it? I wonder if thats something on the new machines?

That is the ring light from Tormach, after years of always being frustrated with shadows being cast directly where I am trying to look... it was a no-brainer. For a cheap Chinese light, it works pretty well.