Author Topic: Finally getting up and running - question on drilling...  (Read 285 times)

Offline Chip Owner

  • Ewok
  • *
  • Posts: 28
    • View Profile
Finally getting up and running - question on drilling...
« on: June 21, 2020, 18:52:53 pm »
While the machine isn't fully finished yet, it is at least cutting now.

Still have to sort the vacuum bed, awaiting delivery of the plastic to cut, blower now installed.

So far small pieces, we work with 1050 aluminium so getting the feeds & speeds sussed is taking time. While I learn, I'm still using the discount, single flute carbide endmills really designed for plastic.

I guess like many, started slow and tentative. Sadly the endmills don't allow any serious depth of cuts at this time so I'm experimenting with speeds. Better cuts today, still not right, DOC 0.08, 16k -18k RPM and 3500mm/m spiral lead in.

Except the initial drill holes, these are drill operation with a spiral drill, 200mm/m doc 0.2mm, same RPM as profile cuts  - 3mm endmill to make a 3.6mm hole.  I did try higher/faster earlier without success. Slowing feed rate down improved a few.

I'm struggling to get a decent hole each time, while there is plenty of info on feeds & speeds for cutting, (albeit for much lighter machines) I'm not seeing much for any drilling operation.

Any tips on drilling with an endmill.

I need to point out, once I get this maching running, constantly changing tools is not an option for productivity. 


Offline Bubba

  • CNC Jedi
  • *****
  • Posts: 2939
    • View Profile
Re: Finally getting up and running - question on drilling...
« Reply #1 on: June 21, 2020, 19:32:45 pm »
Any tips on drilling with an endmill.
******************
There are two options. Because endmills are not designed for plunge drilling so if you wan't plunge drill with, you need hole on center (aprox half diameter of the endmill. Second option is milling a hole with an endmill.
« Last Edit: June 21, 2020, 21:48:15 pm by Bubba »
My 2¢

Win 10 64 bit, CB [1.0} rc 1 64 bit, Mach3, ESS, G540

Offline Garyhlucas

  • CNC Jedi
  • *****
  • Posts: 1366
    • View Profile
Re: Finally getting up and running - question on drilling...
« Reply #2 on: June 21, 2020, 21:16:32 pm »
I hardly ever drill with a drill bit, preferring to spiral mill all the holes of every size down to the tool diameter.  However I always use fog buster style droplet coolant because without lubrication aluminum welds to the bit very easily and you have to go very slow. I keep a container of sodium hydroxide handy. If the bit welds up I toss it in the sodium hydroxide an it come out completely clean without damaging the bit.
Gary H. Lucas

Have you read my blog?
 http://a-little-business.blogspot.com/

Online Bob La Londe

  • CNC Jedi
  • *****
  • Posts: 3953
  • ^ 8.5 pounds on my own hand poured bait.
    • View Profile
    • CNC Molds N Stuff
Re: Finally getting up and running - question on drilling...
« Reply #3 on: June 22, 2020, 01:46:48 am »
I used to spiral interpolate a lot of holes until I realize that drilling is just so darn much faster. it doesn't have to be fast to be faster cuz it only has to travel the depth of the hole not the diameter of the path 57 times.  I hardly ever spiral interpolate holes anymore and last year I probably did almost exclusively spiral interpolation on the little high speed machines. I just had to find drill RPM and feed rate that worked. A big help was learning how to use g73.  I drill with high-quality split point drill bits. Once I have to resharpen them they get tossed in the manual only drill box. in my machine room there are three machines that are pre-loaded with drills and my big mill outside the machine room is also pre-loaded with a bunch of drills.  the only drilling I do with an end Mill is a de-facto ream to make a start for pressing a pin into an undersized hole.
« Last Edit: June 22, 2020, 01:52:49 am by Bob La Londe »
Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com

Online Bob La Londe

  • CNC Jedi
  • *****
  • Posts: 3953
  • ^ 8.5 pounds on my own hand poured bait.
    • View Profile
    • CNC Molds N Stuff
Re: Finally getting up and running - question on drilling...
« Reply #4 on: June 22, 2020, 01:48:01 am »
I should add that most of the holes that I drill are .256 in in diameter and smaller. I can get away with drilling those even on a 24000 RPM machine.
Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com

Offline Chip Owner

  • Ewok
  • *
  • Posts: 28
    • View Profile
Re: Finally getting up and running - question on drilling...
« Reply #5 on: June 22, 2020, 07:18:01 am »
Any tips on drilling with an endmill.
******************
There are two options. Because endmills are not designed for plunge drilling so if you wan't plunge drill with, you need hole on center (aprox half diameter of the endmill. Second option is milling a hole with an endmill.

I think the first version of this in CB had the hole drawn as a pocket, I didn't know about spiral drilling at that point.

Might be worth trying a profile cut again.

Offline Chip Owner

  • Ewok
  • *
  • Posts: 28
    • View Profile
Re: Finally getting up and running - question on drilling...
« Reply #6 on: June 22, 2020, 07:39:03 am »
I hardly ever drill with a drill bit, preferring to spiral mill all the holes of every size down to the tool diameter.  However I always use fog buster style droplet coolant because without lubrication aluminum welds to the bit very easily and you have to go very slow. I keep a container of sodium hydroxide handy. If the bit welds up I toss it in the sodium hydroxide an it come out completely clean without damaging the bit.

The part in the images I posted was the best holes, non since have been anywhere near as tidy.

Typically the rivet holes we use are 4mm or 5mm in most of our products, these are the oddity hence 3.6mm for a screw and the reason I opted to use 3mm end mills for all.

So question is, would switching 4mm end mill help, then most would just be a straight drill.  I will try a profile cut operation in the meantime.

Re misting, it's an option I've considered, I have a mister fitted. The end game has to be 100% dry cuts, as you can see on the table we have film on the alu while machining, film both sides, non of or products receive any surface finishing after production, the shiny mill finish of the 1050 is the look we keep. In an ideal world, we would add powder coat facility too but fitting this machine into our unit was a stretch.

I started hitting them with water/meths mix from a hand spray pump, it started to lift the film and leave water marks on the sheet. So I persevere with perfecting the dry cut. I have noticed as I get nearer the better feed/speed the part is not that hot.

I'm also aware at this moment the bits I'm using aren't designed for this, I'd rather break £1 bits than £60 while learning. With these bits, almost ridiculously shallow cuts seem to be the only option on 1050.


Offline Chip Owner

  • Ewok
  • *
  • Posts: 28
    • View Profile
Re: Finally getting up and running - question on drilling...
« Reply #7 on: June 22, 2020, 07:59:24 am »
I used to spiral interpolate a lot of holes until I realize that drilling is just so darn much faster. it doesn't have to be fast to be faster cuz it only has to travel the depth of the hole not the diameter of the path 57 times.  I hardly ever spiral interpolate holes anymore and last year I probably did almost exclusively spiral interpolation on the little high speed machines. I just had to find drill RPM and feed rate that worked. A big help was learning how to use g73.  I drill with high-quality split point drill bits. Once I have to resharpen them they get tossed in the manual only drill box. in my machine room there are three machines that are pre-loaded with drills and my big mill outside the machine room is also pre-loaded with a bunch of drills.  the only drilling I do with an end Mill is a de-facto ream to make a start for pressing a pin into an undersized hole.

With an ATC, I'd have gone straight for this option, I can dream.

All a compromise at the moment. Manually I can create our products on a guillotine, lever press and hydraulic hole punches pretty fast, with jigs set up for each element. Admittedly the larger centre holes require 2 punch operations and a lot of clean up as the final diameter hydraulic hole punches are crap, with serious burrs as they wear.

 

Offline kvom

  • CNC Jedi
  • *****
  • Posts: 1572
    • View Profile
Re: Finally getting up and running - question on drilling...
« Reply #8 on: June 22, 2020, 13:00:06 pm »
Two flute endmill with air blast or WD40 works well for me, but I use spiral only for holes not covered by drills.

You can also try the trocho pocket MOP that spiral mills round holes at full depth after a center plunge.

Online Bob La Londe

  • CNC Jedi
  • *****
  • Posts: 3953
  • ^ 8.5 pounds on my own hand poured bait.
    • View Profile
    • CNC Molds N Stuff
Re: Finally getting up and running - question on drilling...
« Reply #9 on: June 22, 2020, 16:36:08 pm »
I don't have an ATC on any of my machines, but I do have quick change spindles and pre-measured tools. It makes a huge difference in efficiency.
Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com

Offline Chip Owner

  • Ewok
  • *
  • Posts: 28
    • View Profile
Re: Finally getting up and running - question on drilling...
« Reply #10 on: June 22, 2020, 17:24:34 pm »
Two flute endmill with air blast or WD40 works well for me, but I use spiral only for holes not covered by drills.

You can also try the trocho pocket MOP that spiral mills round holes at full depth after a center plunge.

Cheers I'll look into those.

Offline Chip Owner

  • Ewok
  • *
  • Posts: 28
    • View Profile
Re: Finally getting up and running - question on drilling...
« Reply #11 on: June 22, 2020, 17:30:30 pm »
I don't have an ATC on any of my machines, but I do have quick change spindles and pre-measured tools. It makes a huge difference in efficiency.

Cheers, I'll look into those.

I think I've tested as far as I can with the discount end mills, having blasted through several more test pieces today. 

Offline Chip Owner

  • Ewok
  • *
  • Posts: 28
    • View Profile
Re: Finally getting up and running - question on drilling...
« Reply #12 on: June 25, 2020, 16:43:10 pm »
Resolved with decent endmills!

Significantly more expensive endmills I might add, but they've enabled me to dry cut & drill, thin sheet 1050, little or no post cut cleanup in one pass.

Reduced cutting time to a quarter.

Chip earned his keep today finally.

Next job vac bed.

Online Bob La Londe

  • CNC Jedi
  • *****
  • Posts: 3953
  • ^ 8.5 pounds on my own hand poured bait.
    • View Profile
    • CNC Molds N Stuff
Re: Finally getting up and running - question on drilling...
« Reply #13 on: June 25, 2020, 23:09:55 pm »
I forgot to mention that you can get drill/mills in some sizes.  I find 1/8" (3.175mm) very handy making control panels.  I guess I didn't really pay attention to what type of work you were doing, but they could be quite handy for some things. 

A drill/mill has a pointed tip for drilling and regular mill geometry flutes on the sides.  They are most common with a 90 degree tip so the same tool can also be used for chamfering or edge deburring. 

A drill/mill might wreak havoc on a vacuum bed though. 
« Last Edit: June 25, 2020, 23:12:06 pm by Bob La Londe »
Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com

Offline Chip Owner

  • Ewok
  • *
  • Posts: 28
    • View Profile
Re: Finally getting up and running - question on drilling...
« Reply #14 on: June 26, 2020, 06:58:19 am »
I forgot to mention that you can get drill/mills in some sizes.  I find 1/8" (3.175mm) very handy making control panels.  I guess I didn't really pay attention to what type of work you were doing, but they could be quite handy for some things. 

A drill/mill has a pointed tip for drilling and regular mill geometry flutes on the sides.  They are most common with a 90 degree tip so the same tool can also be used for chamfering or edge deburring. 

A drill/mill might wreak havoc on a vacuum bed though.

These are just ordinary end mills, intended for aluminium, 3mm.
DLC coated on this occasion, I'll probably invest in the 'Superior' version next time.  (LKHtools in UK if anyone interested). Tearing off chips on the 1050 as I'd hoped.

Pressure foot helped too on this occasion just stop the sheet lifting as only bolted down in corners. 850mm x 800mm sheet, I confess to thinking it wouldn't work but surprisingly it did, hovered above the surface at full depth cut, so only came into play if the part did lift, not rubbing all the time.

Vac bed will have an MDF waste board on top to draw through.