• This site uses cookies. By continuing to use this site, you are agreeing to our use of cookies. Learn more.
  • How to Donate to Support the Forum and Upgrade Your Account

    To upgrade your account, click on your name/User ID, and your profile box comes up. On the right side (highlighted above) you will see "Account Upgrades" Click on this, and you will see your upgrade choices:

    * Premium Membership - recurring (12 months, recurring) $25.00 per year This is for one-year premium membership, automatically renews. Less ads, more access.

    *Premium Membership - non-recurring (12 months, non-recurring) $30.00 for 1 year This is for one-year premium membership, does NOT automatically renew. Less ads, more access.

    * Sustaining Membership - recurring (12 months, recurring) $50.00 per year This is for one-year sustaining membership, automatically renews each year. No ads.

    * Sustaining Membership - non-recurring (12 months, non-recurring) $50.00 for 1 year This is for one-year sustaining membership, does not automatically renew each year. No ads.

[4]

Anyone Using a Drill/Mill End Mill?

January Project of the Month [3]
[10] Like what you see?
Click here to donate to this forum and upgrade your account!

ecdez

Active User
Active Member
Joined
Jul 10, 2012
Messages
410
Likes
257
#1
A few weeks ago a local guy gave me a stack of about 20 pieces of 1" thick steel flat bar and needed a 7/8" hole drilled on each end and the end rounded over so I set it up and used progressive drill sizes to get me to 1/2" than used and end mill to bring the hole to size and then shape the perimeter of each end. Didn't think much else of it but today he gave me 20 more so this looks like it's going to be a regular thing. My problem is the tool changes for the drilling operation takes too much hands on time (CNC mill without a tool changer) and I'd like to find a better solution. Was thinking an annular cutter for the hole and then an end mill to get the hole to final size and shape the end and that brings it down to one tool change. I was thinking about the drill/mill tools which would get me down to no tool changes but I've never used one. Anyone have experience with these?

Any better ideas on how to accomplish this seemingly simple task that I've overblown as usual?

It's 1" x 2" hot rolled flat bar with a 7/8" (just over actually) hole and a 2" diameter half circle milled into the end.

Drill/Mill in question would be this one or similar that would accomplish the same.

https://www.mcmaster.com/#2957a17/=1b3o0yk
 

Wreck™Wreck

Active User
H-M Supporter - Sustaining Member
Joined
Sep 29, 2014
Messages
2,009
Likes
1,627
#2
Interpolate the radii on the ends and use a 7/8" drill bit for the holes, does not get much simpler then that.
5 minutes or less per part, at $250.00 per hour shop rate roughly $20.00 per part with Customer Supplied Material. If the Customer requires a fixed tolerance on the hole sizing, say .875 +0.00 -.005" or .875 +.005 -.000 double the price as you will have to ream or bore unless your machine can interpolate a bore within that range.

Have at it.
 

Bob La Londe

Active Member
Active Member
Joined
Apr 19, 2014
Messages
370
Likes
242
#3
My suggestion too. Interpolated spiral milling. Its not as fast as drilling, but it might be faster than multiple tool changes.
 

Boswell

Hobby Machinist since 2010
H-M Supporter - Sustaining Member
Joined
Feb 27, 2014
Messages
418
Likes
126
#4
what about a jig that let you position the parts quickly so you could drill a pilot hole in all 20 pieced, then tool change to a 7/8 bit to drill the hole to size on all 20 then tool change to an end mill to mill the arc. The total tool changes for 20 parts is not very much time per part and if you can get him to send you more than 20 at the time the overhead of tool changes is even less per part. The key to this technique is to be able to clamp the parts in registration quickly.
 

magicniner

Active Member
Active Member
Joined
Oct 21, 2017
Messages
176
Likes
135
#5
My suggestion too. Interpolated spiral milling. Its not as fast as drilling, but it might be faster than multiple tool changes.
Bob has hit the nail on the head here, it's obviously a suggestion based on good knowledge of using a CNC mill.
 

ecdez

Active User
Active Member
Joined
Jul 10, 2012
Messages
410
Likes
257
#6
I agree about the interpolated spiral milling. I use it all the time in aluminum. I seem to have a lot of difficulty when it comes to steel though. Probably my feeds and speeds or machine rigidity or a combination of both. Maybe I'm not pushing it hard enough?

It's worth a shot I'm just not keen on me breaking a $40 end mill. Wouldn't be much different than buying a $40 mill / drill to test it out though.
 

Ray C

H-M Supporter - Sustaining Member
Staff member
H-M Supporter - Sustaining Member
Joined
Nov 16, 2012
Messages
4,614
Likes
291
#7
what about a jig that let you position the parts quickly so you could drill a pilot hole in all 20 pieced, then tool change to a 7/8 bit to drill the hole to size on all 20 then tool change to an end mill to mill the arc. The total tool changes for 20 parts is not very much time per part and if you can get him to send you more than 20 at the time the overhead of tool changes is even less per part. The key to this technique is to be able to clamp the parts in registration quickly.
^^^^^
This is what I would do.

Ray C.
 

ecdez

Active User
Active Member
Joined
Jul 10, 2012
Messages
410
Likes
257
#8
I thought that was a good idea too. Especially if I could pre-drill on a drill press as a pre-op of sorts. The problem is the blanks he gives me are pre-cut to within 1/4" of each other. If I set up a jig so that the holes are X distance from each end then on the longer of the blanks the holes will be too close to the ends when I finish them up on the mill. If there was a hole in only one end then this would be a perfect solution.

I just looked it up and the holes are 0.89" so even if I use a 7/8" drill I still have to finish the hole to size. Not really a problem as I use the same end mill to finish the hole as I do for the arc. The main goal is me trying to reduce the number of tool changes to reduce the hands-on time. I'd prefer to use a single tool so no tool changes just change the part, hit run and walk away for 10 minutes.
 

Bob La Londe

Active Member
Active Member
Joined
Apr 19, 2014
Messages
370
Likes
242
#9
I have spiral milled holes in steel before. Its just about getting the numbers right. Some steel machines better than other steel though. I've found recently for example that 4140HT machines nicer than just about any low-c hot rolled steel. When you are calculating speeds and feeds treat it like ramping into a slot at 100% engagement. Well because, that is what you are doing. I prefer an end mill slightly larger than the radius of the cut, but slightly smaller will also work. Removing a large slug this way however can be a problem, because you can NOT predict what the slug will do when it comes out. I'm a fan of HSM Adviser (FS Adviser is the free version) for calculating speeds and feeds, but I tend to go with reduced tool loads over what Eldar's software tells me. Also, the free version does not to take into account the power curve (dyno chart if you will) of the machine.

As to using a stop why not do all of one end then all of the other end.

A drill press... there you have touched on one of the things I do. On my little high speed mills they tend not to spin slow enough for regular hole drilling and as mentioned interpolated spiral milling is slower than drilling, so I often spiral mill just deep enough to act as a drill guide, and then when the rest of the part is done I drill all the holes on the drill press. .89 is enough larger than .875 to be a concern though.

The thing to think about is how to make the best use of your total net time.

Recently I cut a replacement control panel for a boat. It would have seemed that CNC would be ideal for it. I spent a couple weeks thinking about the best way to do the job. I thought about a couple ways to probe and measure it. I thought about how to turn the panel so it would fit in my work envelope. I thought about indexing it on the mounting screw holes and moving it. Then I said screw this and did it by hand with a bandsaw, nibbler, belt sander and drum sander, and a hand held cordless drill. It took me a few hours, but then I was done and it looked good. I only CNCed the text on the finished panel.

Here is a video of my KMB1 spiral milling a bolt hole in a piece of generic angle iron being made into a vise hold down. I don't recall if that's one of the speeds and feeds I save in my style library or not, but it worked.


As a sort of aside note. That was obviously done with just a little cutting oil. It works. However on my recent excursion into 4140HT (I've spent several weeks working on some specialty press dies with 3D embossing) I have been using altin coated with massive flood with good results. One of the things I am doing on the high speed mills is spiral milling holes from .248 -.252 for alignment pins with a .125 4 flute altin coated end mill at ... 8008 rpm. (8000 is the bottom of my power curve on those machines.) I'll drill and ream to finish.
 
Last edited:

ecdez

Active User
Active Member
Joined
Jul 10, 2012
Messages
410
Likes
257
#10
Thanks for sharing! You got through that material pretty quick too. I use the HSM advisor too; works for what I do here.
 
[6]
[5] [7]