Mic those endmills...

[BobWarfield]

This is probably not strictly a CNC thing, but I discovered it CNC'ing. I was working on parts for Team Build 2, the Comber Rotary. I'm doing bearing blocks. Here are two proto-blocks (not ready for production!):

I got to measuring the parts and discovered they were off by several thou in various odd ways. Eventually I wrote it all down and looked for patterns. The outside profile was too big and the inside pocket was too small. A little later it dawned on me and I went off to mic the diameter of my endmill.

I was expecting 3/16" or 0.1875". Instead I had 0.1837", which looks to me like would account for most of my errors. Gotta run the part and try again, but I was surprised at how far out that endmill was.

Cheers,

BW

 

[Maryak]

Bob,

Somebody must have sharpened the flutes at some stage. ??? ???

Another Bob

 

[DavHJ]

Was the end mill an import? If it was it wouldn't suprise me becouse I've ran into the same thing on my CNC Machine.
I alwayse check the diameter first now and plug that number into the tool diameter offset with good results.
Also I try to use the shortest flute length I can get away with to reduce flex.
Good Luck,

Dave

 

[rake60]

Actually the ANSI tolerances for end mills are not as tight as one might expect.
Depending on the type of end mill it could be as much as .005"

 

[Mike N]

Depending on how rigid your cnc milling machine is, when climb cutting the endmill will push away from your work piece. Usually with a rough cut & one finishing pass (if the end mil is sharp) the cutter should cut to its intended size.

 

[BobWarfield]

The endmill was a name brand, but it was purchased from eBay at a less than half price. It was likely either resharpened or a reject.

These little endmills are cheap enough I may shell out a bit more for one that is accurate. But I do think I'll be mic'ing them as well.

Best,

BW

 

[deere_x475guy]

Funny this post should come up now. Just last week I was using what I thought was a .500 end mill and I used this number for my tool offset. As it turns out the the .5 end mill I chose was .487, apparently this had had the flutes ground at some point. I now mic the end mills.

 

[cfellows]

I've run in to this with end mills bought on ebay. I'm wondering if in some cases metric end mills are being sold as "close enough" inch sizes.

Chuck

 

[Bluechip]

Now you've started something ... :

Been miking my end mills, mostly Far East ... all are 'not to size', some by about +/- 5% on nominal.

But, all my slot drills seem to be spot-on, as well as I can measure, these are all UK made.

So, is it that they are UK made, or do slot drills have to be tighter in tolerance ??

Assuming end mills sort of er ... mill on the end, and slot drills er .. do slots to a specific width ??

Dave

 

[DavHJ]

Bob,

Looking at your parts again it looks like to me that the end mill might be a little dull, too long or feed too fast.
Small dia. carbide end mills are affordable these days you might want to try roughing out with a high speed then finish with a carbide with higher spindle speed. Just a thaught.

Dave

 

[DICKEYBIRD]

Sadly, I don't have a CNC mill but have been cutting out balsa & ply parts for my model aircraft designs since 1998 with a home-built CNC router.

One of my first "school of hard-knocks" lessons was to always accurately measure & record the effective kerf width whenever I changed router bits or made drastic changes in materials; ie: balsa to ply or foam. I measured the width of a piece of stock, cut it into 2 pieces using the new bit, re-measured the combined width of the 2 pieces, subtracted that from the original measurement and that was the effective kerf. It was never the same as the marked size or the measured dia. of the cutter!

 

[raym 11]

How do you mic an end mill and not chance damaging the mic? Odd flute are trickey to calc also?
Ray m

 

[speakerme]

Hello,

Height gage on a granite table works for some 2 flutes, 3 flutes tougher, there is a 3 flute micrometer avail but, as you would expect, expensive.
You can also hand mike a 2 flute if done with care.

I just checked some import sets that I have (never used never sharpened): Nominal 3/4" two flute measures .745 who woulda thunk!

Most of the time it does not affect me much, since I am just using it as a cutting tool, and cutting to a dimension scribed or measured. I can see that would be a real problem in CNC work.

Best Wishes

Chuck M

 

[joeby]

A shop I worked in had a very simple, but very good idea that I haven't seen used since I left there. They had a tool/cutter grinder there, and every machinist was taught to use it. If you dulled an end mill, it was your responsibility to sharpen it. The toolcrib attendant would, as a result, measure each end mill that came into the crib, new or resharpened, and tag it with masking tape marked with the diameter. Made life a lot easier.

Anyway, checking the end mill diameter is a very good idea, especially for critical dimensions. You can buy name-brand end mills that will be very close to size, and some companies will verify the diameter to .0001" on them for a cost. I have had them quoted this way for a job, with the end mills being in the $40-$50 each range for 1/8" end mills.

One other issue affecting size of the workpiece is runout in the toolholder or spindle, or both.

I have gotten in the habit of checking the end mill diameter, and then setting the tool diameter offset a few thousandths larger. Easy to make an adjustment and take more material off, putting material back on is a different matter. There are many ways to avoid running the entire program over if you need to change the offset. I use block delete if the program is short enough, or just add a tool change or line number corresponding to the tool I'm using, that I can easily search for to do a restart.

Kevin