CAMheads CNC Router Forum By: CAMaster CNC

Go Back   CAMheads CNC Router Forum By: CAMaster CNC > Tips & Techniques > metal work

Reply
 
Thread Tools Display Modes
  #1  
Old 04-16-2015, 04:47 PM
Keeley Service Keeley Service is offline
CAMhead Friend
 
Join Date: Oct 2014
Location: Oklahoma City
Posts: 5
Default Help with choice of bit, feed, and speed

I am fairly new to working the machine at our shop, and it seems we may have had some bad advice in the past. We are cutting aluminum cases for guitar effects pedals, and have been using a 1/2" carbide end mill in a simple plunge to drill some of the holes. Speed 13,000, feed 8. This has resulted in a lot of chipped bits, costing at least $100 each time.

I spoke with Onsrud (most of our bits come from them) about the best course of action to prevent this, and the tech asked me why the hell we were using a router bit to drill. I'm just doing what the guy before me did. I have tried to use a 1/2" drill bit, but can't seem to find the right feed and speed to drill clean holes without burrs.

We have a Stinger I with 1.7 kw spindle and Mister. The aluminum is 1/16" thick. Can an experienced and knowledgeable machinist recommend a cost-effective drill bit, and some feeds and speeds for me? Thank you all for any help you can provide.
Reply With Quote
  #2  
Old 04-16-2015, 04:59 PM
Gary Campbell's Avatar
Gary Campbell Gary Campbell is online now
CNC Tech & Trainer
 
Join Date: Dec 2012
Location: Marquette, MI USA
Posts: 2,765
Default

I suggest that you use a 1/4" single O flute bit on an inside profile toolpath with spiral (.030" pass depth) strategy and machine these holes. Feeds XYZ=30ipm, rpm 13500. Your material, bits and machine will thank you.

You can see the process here, albeit on much thicker material: https://www.youtube.com/watch?v=_38rxqSn0yk
__________________
Gary Campbell
CNC Technology and Training
The Ultimate Woodworking Machine
GCnC411@gmail.com
https://www.youtube.com/user/Islaww1/videos

"There are 10 kinds of people in the world. Those that understand binary logic, and those who don't"
Reply With Quote
  #3  
Old 04-16-2015, 06:34 PM
Keeley Service Keeley Service is offline
CAMhead Friend
 
Join Date: Oct 2014
Location: Oklahoma City
Posts: 5
Default

Thank you, Gary. Would it be impractical to do this with a 3/16 bit? We have plenty of those, but no 1/4 bits. Does it have to do with the bit being at least half the diameter of the hole being cut?
Reply With Quote
  #4  
Old 04-16-2015, 07:58 PM
Gary Campbell's Avatar
Gary Campbell Gary Campbell is online now
CNC Tech & Trainer
 
Join Date: Dec 2012
Location: Marquette, MI USA
Posts: 2,765
Default

Keeley...
There should be no problem, but you may fling a little 1/8" slug every now and then. Same feeds/speeds for the 3/16, if its a single flute
__________________
Gary Campbell
CNC Technology and Training
The Ultimate Woodworking Machine
GCnC411@gmail.com
https://www.youtube.com/user/Islaww1/videos

"There are 10 kinds of people in the world. Those that understand binary logic, and those who don't"
Reply With Quote
  #5  
Old 04-16-2015, 10:40 PM
TinKnocker TinKnocker is offline
CAMaster owner
 
Join Date: Jun 2014
Location: MD
Posts: 280
Default

Gary is correct. You could also do the same thing with a 3/16 or 1/4" endmill. A half inch hole is a huge hole to drill in .063 aluminum. Typically if you try to go straight through with such a large diameter bit the tip of the bit clears through the sheet before the tips of the flutes and exerts a heavy lifting force on the metal, and a lot of times you'll end up with trianglish holes. Another option would be to cut smaller holes and then open them up after the fact with a drill press. If you go that route I would climb the bits up about a 16th at a time and clamp it well because a half inch drill puts a ton of torque on a part, and spinning sheet metal plays hell on the hands.
__________________
-PETE MALONE

SR-34
V-Carve Pro V8
1.7kw Spindle, FTC and counter balance and T-rails
Recoil Ready
Reply With Quote
  #6  
Old 04-17-2015, 12:10 PM
Keeley Service Keeley Service is offline
CAMhead Friend
 
Join Date: Oct 2014
Location: Oklahoma City
Posts: 5
Default

I appreciate all of your inputs. We use the 3/16 single flute bits for the routing ops on the rest of the cases, and when it cuts the main hole for the switch (0.52"), it flings the small slug. That's fine with me, I would be happy to cut the other holes like this rather than using the drill bit. What I am most concerned about is the shape of the hole. As you can see in the photo, it is not round. All of the routed holes are like this, but they have not always been.

It does not matter if the bit is old or new, or how much mist is flowing. Is this more of the same--feed and speed?

Also, our production numbers are high enough that we don't want to add another step by using the drill press--we got the Stinger to take care of all the operations in one station. The boss wants to double our current production, and we need to make the process faster and more reliable.
Attached Images
File Type: jpg photo (1).jpg (44.4 KB, 58 views)
Reply With Quote
  #7  
Old 04-17-2015, 12:48 PM
Gary Campbell's Avatar
Gary Campbell Gary Campbell is online now
CNC Tech & Trainer
 
Join Date: Dec 2012
Location: Marquette, MI USA
Posts: 2,765
Default

Keeley...
There are really only 2 causes for your out of round condition.

1) Excessive lash in the drive mechanics (maintenance adjustment)

2) Toolpath parameters that develop force beyond what the machine electro-mechanics can contain.

There is a third possibility: 1 caused by 2

Solution: Clean, Lubricate and Adjust drive system. Adjust feeds and speeds that are appropriate for machine.
__________________
Gary Campbell
CNC Technology and Training
The Ultimate Woodworking Machine
GCnC411@gmail.com
https://www.youtube.com/user/Islaww1/videos

"There are 10 kinds of people in the world. Those that understand binary logic, and those who don't"
Reply With Quote
  #8  
Old 04-17-2015, 01:32 PM
TinKnocker TinKnocker is offline
CAMaster owner
 
Join Date: Jun 2014
Location: MD
Posts: 280
Default

Is that picture from a pocket toolpath or from a 1/2" drill attempt?
__________________
-PETE MALONE

SR-34
V-Carve Pro V8
1.7kw Spindle, FTC and counter balance and T-rails
Recoil Ready
Reply With Quote
  #9  
Old 04-17-2015, 05:27 PM
Keeley Service Keeley Service is offline
CAMhead Friend
 
Join Date: Oct 2014
Location: Oklahoma City
Posts: 5
Default

1/2" profile with 3/16" bit. 13,000 at z 8, x and y 15, ramped.
Reply With Quote
  #10  
Old 04-24-2015, 02:14 PM
Keeley Service Keeley Service is offline
CAMhead Friend
 
Join Date: Oct 2014
Location: Oklahoma City
Posts: 5
Default

I have found one of the major problems with my circles--the Y-axis belt drive gear has some play on its axle, and I am removing the transmission mounting plate to tighten everything down.

Can anyone tell me what type of red lube is sandwiched between the face-to-face aluminum sliding surfaces? I may need to go buy some locally before I can get back to machining. Thanks for the help.
Reply With Quote
Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off

Forum Jump


All times are GMT -4. The time now is 10:29 PM.


Powered by vBulletin® Version 3.8.4
Copyright ©2000 - 2018, Jelsoft Enterprises Ltd.