I have a question I have a job coming up that has approximately 400 holes .500 deep with a tolerance of +/-.0003 on diameter and .0005 from hole to hole, I'm thinking that using a boring head will be better to hold the hole size and location, I was planning on using the end mill to rough the holes to size leaving .010 stock on the diameter then finish them with the boring head. my boss says no he wants them circular milled using a stubby 3/8" carbide end mill cause it will be faster, I will give him that it will be faster but I don't think the results will be as good I am doing this on a HAAS VF3 YT vertical mill. Any suggestions or comments will be appreciated.
Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
Boring vs Circular Milling
- Thread starter cncguy51
- Start date
- Replies 40
- Views 10,522
Spinit
Titanium
- Joined
- May 13, 2007
- Location
- Central Texas
Well to me it seems that each hole in relation to the other being .0005 is no problem interpolating it you c drill drill shallow then go in and rough it carefully then finish with another emill. I would frefer to do that myself because with boring each one there will be biuldup of stringy stuff which interpolation and coolant will eliminate and you have +-.003 on the diameter. If actual the .0005 tolerance is really just somewhere even if you go nominal. The intent of the tolerance looks to me to be relative being given a break on the Hole diameter tolerance.
manualmachinist
Stainless
- Joined
- Oct 5, 2012
- Location
- Battleground, Washington
I thought I read +-.0003" from the OP.
Since I'm a complete newbie to CNC I have often wondered how close circular interpolation could hold vs boring to generate a true circle. I will be watching this thread to see what the experts say.
Mike1974
Diamond
- Joined
- Nov 5, 2014
- Location
- Tampa area
Are you going to check these with tenth gage pins? You will see how accurate your machine is real fast if so. I am not saying you can't do it, but +-.0003" may be problematic. I will say I have interpolated small holes (8mm'ish) on an old Matsuura and it was holding tenths according to my tenth pins. The problem I had was taper, we ended up milling them about .0003" under and honing them in.
For the record, it was just 3 holes in 3 or 4 pieces, not nearly what you need to do quantity wise.
For the record, it was just 3 holes in 3 or 4 pieces, not nearly what you need to do quantity wise.
Joe Miranda
Titanium
- Joined
- Oct 19, 2004
- Location
- Elyria Ohio
I would never circular mill holes with that close of tolerances unless I got write-off from the customer. That being said, I worked for a guy about 6 years ago that wanted me to circular mill holes like that all day long. It never came back to bite us but it was for work that was used in-house.
Rob F.
Diamond
- Joined
- Aug 5, 2012
- Location
- California, Central Coast
What is dia. of the hole? I see qty 400, .500 deep, +-.0003.
You better make sure that your leadscrews and nuts have minimum reversal error for interpolation to that tolerance. If the machine is worn in the middle of its travel envelope, you might have a hard time holding +/- .0003 on diameter. I agree that milling the hole is faster, but only if you don't have to do the job twice.
The hole size is .5007-.5013, our machine has a renishaw probe on it and that is what we use to check the hole diameters, I also check them with a couple of gage pins (GO .5006/ NO-GO.5013), taper is one of the things that I am concerned with also, once the end mill starts to taper then I will have to change the tool and then tweak it back out to the proper size and continue from there, so in the long run I don't really see where I will be saving anytime over boring them.
upnorth5axis
Hot Rolled
- Joined
- Aug 20, 2013
- Location
- upper michigan
material Type? Either way will work but depends on machine. Boss pays the bills so I guess your going to endmill them
athack
Stainless
- Joined
- Nov 2, 2009
- Location
- Michigan USA
If it comes down to it and the customer checks the holes with the proper gages you're going to have a problem. Gage pins can not measure in tenths. A probe usually runs out too much to check a diameter that precise. Roundness taper bow all come into play. If the holes are through holes, 1/2 deep is stated but does not say bottom hole, a single pass hone tool added at the end would work wonderfully for achieving diameter roundness and straightness.
Athack
Athack
gustafson
Diamond
- Joined
- Sep 4, 2002
- Location
- People's Republic
Any reason not to ream them?
Never had much luck with reaming holes to that tight of tolerance.
The holes are 1.25 deep thru holes with the top part of the hole bored .50 deep with 1/2-13 threads the rest of the way thru, we will tap the holes from the back .75-.80" deep then flip the plate over and machine the holes from the face as to not get any thread marks in the .501 +/-.0003 hole.
I didn't know they made a hone for a mill? Where would I go about looking into one of those for our machine athack?
The holes are 1.25 deep thru holes with the top part of the hole bored .50 deep with 1/2-13 threads the rest of the way thru, we will tap the holes from the back .75-.80" deep then flip the plate over and machine the holes from the face as to not get any thread marks in the .501 +/-.0003 hole.
I didn't know they made a hone for a mill? Where would I go about looking into one of those for our machine athack?
Mike1974
Diamond
- Joined
- Nov 5, 2014
- Location
- Tampa area
You know they make tenth gage pins, right? A probe runs out too much?!? WTH, the probe in my machine is indicated to about .0001" runout, and I do regularly check it to be sure. To be clear if a plus .5000 gage pin goes in, the hole is bigger than .5000, but you can always go to the .5002 gage pin and see if that one goes in, if it doesn't your hole is likely .5001 or .5002. ...
gustafson
Diamond
- Joined
- Sep 4, 2002
- Location
- People's Republic
If you keep your process consistent reaming is the way to do it. you just need the right size reamer and a reliable starting diameter and consistent lubrication. I would be surprised if a reamer that reams one hole at .501 will not continue to do so under the same circumstances.
Drill 1/2 tap drill.
interpolate the .501 x.5 dp to, for instance .498.
ream it with a proven good .501 reamer
A 501 reamer may not ream 501 spot on, but with a given chip load and lube level, i will bet it will give you the same size hole 400 times, so the question is to find the chip load, and starting reamer diameter, maybe it is .5005 or........
Drill 1/2 tap drill.
interpolate the .501 x.5 dp to, for instance .498.
ream it with a proven good .501 reamer
A 501 reamer may not ream 501 spot on, but with a given chip load and lube level, i will bet it will give you the same size hole 400 times, so the question is to find the chip load, and starting reamer diameter, maybe it is .5005 or........
DMF_TomB
Diamond
- Joined
- Dec 13, 2008
- Location
- Rochester, NY, USA
.
do what your boss wants. it never usually pays to argue with the guy deciding on your pay rate and if you keep you job another week.
Bill Jackson
Plastic
- Joined
- Mar 25, 2015
Burnishing tool?
Hello 1982
Reamer would be my absolute last choice. Use an Endmill! For 2 reasons, it will be faster, and your boss said to do it this way!
IeliteENGINEER
Cast Iron
- Joined
- Sep 23, 2013
- Location
- N IRELAND
Would a boring head hold that tight on production runs? I don't think any of these methods is robust enough for production hitting that tolerance, you would be setting your boring head more or less every 50 holes and your end mill you would be fighting wear taper and any small amounts of backlash in the screws. You could look a reamer and leave a very fine amount on to ream off even run a semi finish reamer and then finish it. Standing at the mill fighting a part all way home costs a ton of money as well you want to set up hit start and have the parts come out perfect. A reamer might not be the answer but there must be something you can buy?
gustafson
Diamond
- Joined
- Sep 4, 2002
- Location
- People's Republic
Hello 1982
Use an Endmill! For 2 reasons, it will be faster, and your boss said to do it this way!
not with the tolerance you won't
