Center Drill Help

[motor-vater]

tried a search but most of the info is pretty dated so links not working, etc. What is the secret to perfect center drill depths. I seem to find lately that no 2 centerdrills are the same and when I try to modify existing geometries from the library it starts to get dicey at best. Verify does not seem like a reliable resource for validating drilling depths. What am I missing here? Is Gcodes old chart still floating around somewhere? or is there a way to truly define geometries in master cam and use the hole diameter to calculate depth? I'm stumped?? Thanks as always

[Colin Gilchrist]

6 minutes ago, motor-vater said:

tried a search but most of the info is pretty dated so links not working, etc. What is the secret to perfect center drill depths. I seem to find lately that no 2 centerdrills are the same and when I try to modify existing geometries from the library it starts to get dicey at best. Verify does not seem like a reliable resource for validating drilling depths. What am I missing here? Is Gcodes old chart still floating around somewhere? or is there a way to truly define geometries in master cam and use the hole diameter to calculate depth? I'm stumped?? Thanks as always

Personally, I try to avoid true Center Drills wherever possible, since the tip length does vary between tools. I prefer a true Spot Drill. I will usually go with the same angle as my drill tip. Harvey Tool makes 60, 82, 90, 100, 120, 130, 140, 150, and 170 degree tip angles. So you're sure to find something to fit your needs. Plus, the tools have a fairly tight tolerance on tip angle and diameter, so you'll only have to model it once...

[jlw™]

+1 to that.  I am stuck with what is in the dispenser but I have it modeled accurately and use it every time.  I spent about 20 minutes after every one left one day testing the 3 different spot drill we have to get the result in the machine to match the output from Mastercam.

I also do the same with threadmills... particularly NPT.  We just got a whole bunch of different NPT threadmills so I'll be starting over on that one.

[motor-vater]

I too like spot drills, guess I got drawn twords the center drill because its a reprogramming job where they previously used a 90 deg center drill so they could break the edge and drill some pretty small long holes with a .001 true position tolerance. I figured if that wasn't broke dont try to fix it. lol But I guess its my job to optimize this bad boy. Originally the job came to the shop years ago with a program already in place and a whole box full of custom tools. I spent most of the day scratching my head wondering what in the hell were they thinking. Over the years its gotten pretty hacked and chopped so it hit my desk as a reprogram and organize deal. But boss said this is one of the jobs that doesnt matter how long it runs as long as the parts are perfect. Funny thing is I looked at it and said oh this should be ez.... lol then I saw all the tools, blue print and old program and was like WOW did this just get hard, or was someone really just overthinking this thing... lol Guess we will find out tomorrow when the chips start flying

[motor-vater]

question though, if you guys had to drill a bunch of .118 through holes in 4340 .300 deep with a +or- .002diameter and a .001 true position tolerance. what would your process be. the previous program starts with a comment to remove backlash?, then center drills, pecks at .020ish with a drill, then pecks with a 3mm ball end mill, and then reams it. this process really distracted me and through me off my game, I have never seen someone working so hard to drill a hole. Was it really that hard in the 90's?

[Colin Gilchrist]

Yes, probably that hard in the 90's for someone who didn't really know what they were doing.

Here is what I would do. I'm guessing you want a "90 degree" chamfer left on the part?

I would spot with this tool:

https://us.mikrontool.com/en/Products/CrazyDrill-Twicenter/Articles/CrazyDrill-Twicenter-90/ID/(id)/2.CC.60100.90/(m)/inch

Then I would drill 100's of holes with this, using through coolant, and no peck:

https://us.mikrontool.com/en/Products/CrazyDrill-Cool/Articles/CrazyDrill-Cool-6-x-d-coated/ID/(id)/2.CD.060300.CS/(m)/inch

If, by some unfortunate circumstance, you don't have through coolant, then go with this one:

https://us.mikrontool.com/en/Products/CrazyDrill-Steel/Articles/CrazyDrill-Steel-4-x-d/ID/(id)/2.CD.040300.S/(m)/inch

 

[Colin Gilchrist]

Scratch that.

Pete,

You can do the entire process with one tool, if you only have to go .300 deep:

https://us.mikrontool.com/en/Products/CrazyDrill-Coolpilot/Articles/CrazyDrill-Coolpilot/ID/(id)/2.PD.03000.090.IC/(m)/inch

It really depends on if you can go "deeper" than .300, or if that is the max. If you can get away with .400 (to the tip of the point), then you could do the entire hole in 1 shot...

Otherwise, use a Spot Drill to get your Chamfer and Spot Point, then use the Pilot Drill to poke the .118 hole.

I've held +-.0005 with these drills in Ti and Stainless, all day long. No need to ream.

[nickbe10]

The Mikron stuff is great, also Sphinx (through Big Kaiser). Different lengths and diameters from Mikron so always worth looking at both.

We use these brands exclusively for small holes now (also 3 flute for Al) anything up to 12D and as Colin says deadly reliable and accurate. Watching a 12D .075 drill break through with a burst of coolant at 16 ipm in 15-5 never seems to get old....

[motor-vater]

Colin not sure how you retain so much information and find the time to share it, but you are the man. I programmed it both ways and literally went from 48 minutes to 25.. this includes some pocketing. I got the tool crib to get me some quotes because there is more than one size hole I'm drilling, after that I need approval. man working for someone else is exhausting... If this was one of my jobs in my old shop it would be a no brainier. The other factor will be getting the production coordinator to give me one of the mori's with thru spindle coolant to really capitalize on this plan. Basically I'm saying Thank you

[motor-vater]

Ok So could not get the boss to clear me for the mikron drills. But we do have some of these guhring's laying around the shop

http://www.guhring.com/ProductsServices/SizeDetails?Series=6401&EDP=9064010030000

These holes I need to drill are about .700 deep, break through in Heat Treated 4340. Honestly Im at a loss as to how hard I should run these? Guhring website recommends some pretty ludicrous Speeds, somewhere in the neighborhood off 200 SFM and .0074 chipload. Anybody got any recommendations that might not end up in catastrophic failure? Peck drill? at what depth? etc. I spent the whole day trying to make holes in this stuff, the way it was programmed, the center drill idea is now dead in the water, cause well that just did not work, I think it hurts more than helps. But after an exhausting search of the entire tool crib I could not find 1 stub with a 140 deg tip to spot with. I will order one but the boss thinks Ill be fine without it. Man days like this are challenging, but if that machine sits any longer I'm in trouble. 9 holes in a circular pattern, .001 true position off a pre-existing center hole..... its laughing at me! I still havnt ruled backlash out of the equation.... Thinking about spotting 1 at a time from a reference point in an attempt to combat that, but then again I might just be going insane. Never thought this would be so hard...... But next on my todo list is just punch these suckers in with these better drills and see where that lands me.... Any help is much appreciated

[K2csq7]

With the .001" positioning call, and the tight tolerance on the diameter (no max material allowance) unless your machine is dead nuts... hitting the diameters is the least of your worries. 

Go home in XY, spot 1 hole, go home in XY, spot hole #2, go home in XY, spot hole #3...... also go home before drilling each hole. Machines are much more accurate with repeatability than they are with random positioning. 

[neurosis]

14 minutes ago, K2csq7 said:

With the .001" positioning call, and the tight tolerance on the diameter (no max material allowance) unless your machine is dead nuts... hitting the diameters is the least of your worries. 

Go home in XY, spot 1 hole, go home in XY, spot hole #2, go home in XY, spot hole #3...... also go home before drilling each hole. Machines are much more accurate with repeatability than they are with random positioning. 

I usually just create a point tool path to lead in to each hole from the same direction at a 45 degree angle at a feed.  We are running some parts now that have a 0 true position call out with max material condition and a + .001 -.000 hole diameter tolerance.  We have to keep the parts in QC so they stay at temp and bring them out one at a time to machine.  It's a pain in the A. 

[K2csq7]

Oh, and when you're picking up the datum the true position is called from, ensure you move each axis from home in only 1 direction...... 

What I used to do is pickup the center hole, set my work offset, send the machine home, then MDI G0 G90 G54 X0. Y0. and check the location, make G54 adjustments and repeat the process until that MDI command puts the machine dead nuts on the hole. 

Also, keep the rapid override the same during the MDI command as you will have it when running the program......

(I drove a lot of loose machines) :rollseyes:

[Colin Gilchrist]

On ‎9‎/‎11‎/‎2018 at 7:32 PM, motor-vater said:

Colin not sure how you retain so much information and find the time to share it, but you are the man. I programmed it both ways and literally went from 48 minutes to 25.. this includes some pocketing. I got the tool crib to get me some quotes because there is more than one size hole I'm drilling, after that I need approval. man working for someone else is exhausting... If this was one of my jobs in my old shop it would be a no brainier. The other factor will be getting the production coordinator to give me one of the mori's with thru spindle coolant to really capitalize on this plan. Basically I'm saying Thank you

Thanks for the compliment Pete. I don't know how I retain it all, but I suspect that it has a lot to do with learning to read book when I was a young kid. I really struggled at first, due to the fact that I have dyslexia. In the 3rd grade, I was put into a program for "slow" learners. That really sucked, because my best friend at the time was a kid named Rob Foley, who lived a half block away down my street. We hung out together every day, but stopped hanging out when I got put in that program, because our Elementary School was being remodeled, and they separated our classes. Because he was in the "normal" class, he went to Sunset Elementary, and I got shipped off to Parkwood Elementary for two years.

I struggled with reversing B's and D's, and 6's and 9's especially. The turning point came for me because I have an extraordinary Mother. She read to me almost every night when I was young. We started with some easy books, but I really got hooked on the Hobbit, and Lord of the Rings. At that point, I actually wanted to start reading some stories on my own, but I struggled with reading comprehension and vocabulary. The first books that I was able to read on my own and enjoy were the Hardy Boys. As silly as those stories seem now, they really helped me learn to read on my own, and most importantly, to enjoy reading for pleasure.

By the time I was in 6th grade, I was reading a lot of Steven King. I read "It" during the summer before 7th grade. That's over 1,000 pages, and I ripped through those pages because the story sucked me in, and I couldn't wait to find out what was going to happen next. Without that shift in my mindset, I might never have gotten out of my special classes, and I might have accepted the labels that other people put on me.

When it comes to retaining the information, I really feel like flexing my brainpower through reading has a lot to do with my ability to store and retrieve information. The scary thing is; I'm still learning. I try and make sure that I'm learning something new almost every day. I am always reading, and thinking, and looking for ways to both apply and share what I've learned with others. I really enjoy teaching, because I've had so many great teachers and I'll be forever in their debt. Sharing my knowledge is my way of giving back for how blessed I've been.

[motor-vater]

10 hours ago, Colin Gilchrist said:

I struggled with reversing B's and D's, and 6's and 9's especially.

Obviously G's and M's were never a problem... lol But seriously this website is the greatest source of information for people like me. Thanks to guys like youself, JParis, Gcode, and dozens of other grammer's that are willing to share what they know in an almost 911 rapid response fashion I have always been able to source the experiance and guidance I need to keep food on the familys table.

[motor-vater]

Thank you K2 and Neurosis, I actually never even though about that until your post. While they were running the first part of the day, I actually broke down the drilling cycles with points paths inbetween each hole, so that every hole started with a positive Y move followed by a positive X move directly to the position of the hole. It looks amazing and my boss walked by and stopped in amazement.. lol He was like "thats some old school precision stuff right there" He seemed impressed that I knew about that.. Lol so to you gents I owe the credit.. But I have not needed to use it yet. First 2 parts came out with in the .001 tolerance, by simply removing the center drill and increasing the peck depth.. So now they are sitting in inspection waiting for the buyoff. Good news is I have the secret weapon programmed for tomorrow if by some reason it doesnt make the grade. I bought myself some time! Tomorrow I will have my 140 deg spot drill, and point paths in place should I need them. Thank you guys. I could still use some good feeds and speeds tho. 3 mm guhring drill bit, I went real conservative by their standards anyway. 100SFM with a .003 chipload and a .050 peck. I feel like I could push it harder but I am waiting for experience to chime in.

[Colin Gilchrist]

The SFM for 4340 varies wildly, depending on the hardness and temper condition of the part. For 40 Rc and under, I'd say 200-400 SFM isn't unreasonable. It also depends on how many parts you have to make. The lower the SFM, in general, the slower the cut, but the better the tool life.

As you get above 40 Rc, the SFM becomes a bigger consideration. I had some parta that were about 48 Rc, and I had good tool life at 120 SFM. So 100 is conservative, but no reason to push these tools hard, since your diameter is so small, and the tolerances are tight on both size and position.

I've milled 42 Rc 4340 at 640 SFM, with coated carbide, that had differential pitch and helix on the flutes. (.500 Em, .025 stepover, dynamic milling, flood coolant.)

With such short holes (.118 dia x .300 deep), your biggest challenge is getting coolant on the drill tip, not chip jamming in the flutes. You could easily drill the hole in 1 shot, provided you had thru tool coolant. Without thru tool, I'd consider going to a peck of .100 or even .150. The hole just isn't deep enough to where pecking is 100% necessary. But I also like to push the envelope, so take it with a grain of salt. Your Guhring dril is carbide, correct? 2 pecks per hole should be plenty, and means 2 pecks instead of 6.

My go-to chipload for carbide drills is 2% diameter per tooth, with carbide, for a conservative feed. Looks like Guhring is recommending about 3% DpT. That's not unreasonable for a carbide drill. You could do .005 per revolution easily. At 2% FpT, that's .00472 per Rev. So backing off to .004 is reasonable. The reality is you could easily do double that, at .008 per rev. The only thing that might suffer is finish and tool life. I bet you'd still hit size at that feedrate. The positioning is all about how you approach the holes, which you've got covered.

[Leon82]

For removing back lash we used the approach in ref points. The bossman wanted one axis at a time "loaded" so our dealer coded the post to do that when the rep point was used.

 

I used incremental and when I indicated the face of the part I used the same increment to load the screw

 

Matsuura has an option for g60 single direction positioning

 

On our makino I used the one touch custom button to make a screw load indicate program. But that machine is a thermal growth Trainwreck 

[K2csq7]

11 hours ago, motor-vater said:

First 2 parts came out with in the .001 tolerance,

Friggin kids these days with their fancy new computer machines. 

 

When I was a kid, I had to move each axis in one direction..... uphill, both ways, in a heat wave blizzard.