What's new
What's new

CNC holes are widening

Boltman89

Plastic
Joined
Mar 27, 2020
Hi all, this is my first time posting. I'm working on some high tolerance parts and they have been going well, but the last two i did, began milling two counter bores wider than they have been. I know it can't be that the endmill is wearing out, because that would make the holes smaller. what could be my problem? could there be debris in my tool holder that is throwing the tool off just enough?

Thank you.
 
You're going to need to provide a lot more information.

Machine you're working on. Material you're cutting. Coolant (flood? mist? dry?). Define "wider"... Oval, as in wider from left/right than top/bottom? Just larger in diameter but still round? How much is "wider"? .001" .0001"? .005"?

The less we have to guess at what your problem looks like, the less we have to guess at what your solution looks like.

Plus, a lot of the more experienced guys here don't even feel like trying to help guys who can't be bothered to provide basic information about their problem, so you lose out on decades, if not centuries of experience when they just decide to bypass your thread entirely.
 
Did you bend your mill? Is it in a collet or rigid holder? Many times tool concentricity takes a back seat to cutting diameter.
 
Hi all, this is my first time posting. I'm working on some high tolerance parts and they have been going well, but the last two i did, began milling two counter bores wider than they have been. I know it can't be that the endmill is wearing out, because that would make the holes smaller. what could be my problem? could there be debris in my tool holder that is throwing the tool off just enough?

Thank you.

.
milling aluminum dry you can get material sticking to cutting edge. false cutting edge buildup can cut extra, tends to be unstable as it breaks off and reforms and surface finish is much rougher.
.
tool deflects depending on cutter sharpness and how much cutting. you can mill more (on some parts) if there is less material to mill off as cutter is deflecting less. not unusual to take a semifinish cut so final finish cut is taking a more consistent amount so tool deflection is consistent.
.
if you recut finish cut and it removes more material thats usually a sign you have tool deflection. a dull cutter rerunning
sometimes can take a lot more than expected. just saying sharp and dull tool usually acts different
 
Did anyone adjust backlash compensation recently? Any crashes in the long axis? Shifting workpiece during machining due to poor fixturing?

Does your facility have gremlins, and have they been fed after midnight?
 
Sorry, I work in a small shop and i am not a fully trained Machinist. My boss is teaching me and I'm hopefully going back to school soon, so my knowledge on the subject is limited. at the present, I can set up programs with SolidWorks, and I can do some troubleshooting, but again, my knowledge is limited. I don't even know how I should ask my questions.

machine is a Supermax Max-4XP with a Fanuc O-M CNC. Material is 7075 Aluminum. coolant is mist. Counter Bores are supposed to be .472 in diameter with a tolerance of +.002/-.000. they are wider around completely. I started today and they were coming out well within specs, but the last one i did came out at .475 and the two before that were right at .474, so something changed within the last few parts.
 
Did anyone adjust backlash compensation recently? Any crashes in the long axis? Shifting workpiece during machining due to poor fixturing?

Does your facility have gremlins, and have they been fed after midnight?

not sure if the Gremlins were fed, but they did get a nice bath.

there have been no changes to the machine. I'm the only one who has used it since yesterday, and the first part came out just fine today.
 
.
milling aluminum dry you can get material sticking to cutting edge. false cutting edge buildup can cut extra, tends to be unstable as it breaks off and reforms and surface finish is much rougher.
.
tool deflects depending on cutter sharpness and how much cutting. you can mill more (on some parts) if there is less material to mill off as cutter is deflecting less. not unusual to take a semifinish cut so final finish cut is taking a more consistent amount so tool deflection is consistent.
.
if you recut finish cut and it removes more material thats usually a sign you have tool deflection. a dull cutter rerunning
sometimes can take a lot more than expected. just saying sharp and dull tool usually acts different

looked at the endmill and compared it to a new one and it does seem pretty dull in comparison. it did seem like there was more material clinging to it, even with the coolant on it (mist). definitely doesn't feel like i could cut myself on the teeth. I'll try swapping it out and see how that works.
 
Sometimes you'll notice dimensional changes after a machine warms up. If the tool looks good, comp it and keep making chips.
 
The VERY FIRST thing I would check when an interpolated hole goes oversize.

The taper, and the tool holders. ALL OF THEM.

Nothing can screw up your day more than a chip getting in your taper.
Even worse when it sometimes sticks to the tool, and sometimes the taper,
so you can't instantly nail it down.

I have a scrap casting sitting under the workbench as a reminder. An expensive one. One
little chip turned a $7500 job into a $5000 job when one fricken bearing
hole went .001" over. Now when its a big dollar part, I usually run test pieces right
before running the real thing so that I KNOW that hole is going to be right.


As for built up edge. 7000 series, pretty hard stuff, and it really doesn't melt and
smear like 6061 does. I've never had a melt down in 7075. I personally don't think
its built up edge. If your material was 6061, I'd consider it a possibility especially
running a mist.
 
Did anyone adjust backlash compensation recently? Any crashes in the long axis? Shifting workpiece during machining due to poor fixturing?

Does your facility have gremlins, and have they been fed after midnight?


This isn't THAT thread.... :skep:



A dull tool and MIST, trying to hold +/- .001?

Save the mist for general work in steel.
Flood the alum!

Personally, if I'm gunna not run it dry - I'd flood it all, but ....



---------------

Think Snow Eh!
Ox
 
To add: What feed/speed rates? Tool diameter? 1,2,3,4 flute?

I agree on the flooding, hot aluminum sticks to everything! I find the hard aluminum cuts at a higher feed and speed than anticipated - after-all I even have hand machined aluminum with standard woodworking tools. When I was an apprentice, my day job was in construction. We had a shop job that required a metric-ton of 2x2" 6061 aluminum bars be cut into 4" sections for the mill. My mentor told me how to the drop band saw was going to cut xx pcs in xx time etc etc. I sat through exactly one piece, went to my work truck, chucked a 14" rough carbide framing blade in the beater rough-cut Ryobi miter saw (it only registers 90°, been dropped so many times the miter handle has been missing years). Set it on the tailgate, and took out the material roller tripods, set the 24' raw material on the rollers. He looked at me like I had 11 foreheads as I started 4" drops were coming off the saw as quickly was it were 2x2" wood studs lol.

Also, when running parts as a new machinist, program your holes undersized when they are -.xxx +.000, then spring pass them as needed until you dial it in. You know the rule: "You can always subtract material easier than you can add it."

I find it odd that you had it dialed in, then it moved, now you are saying it was good then moved again? That's more likely a vice/jaw/fixture/tool-holder issue.
 
looked at the endmill and compared it to a new one and it does seem pretty dull in comparison. it did seem like there was more material clinging to it, even with the coolant on it (mist). definitely doesn't feel like i could cut myself on the teeth. I'll try swapping it out and see how that works.
.
1) usually end mills made for aluminum are sharper edge rake/clearance and work better than general purpose mills. its bad when end mill dull and aluminum sticks to cutting edge so bad you getting a hammer and screwdriver to knock buildup off
.
2) sometimes end mill corners get abrasive wear and bottom of bore is smaller. if you check bore with pin or plug gage and it starts in but doesnt go to bottom of bore, bore is tapered, same with checking keyways you check top to bottom looking for taper usually
.
3) when you double end mill stickout amount tool deflection increases 2x2x2 or 8x more. so if end mill stickout of tool holder amount changes it easily effects tool deflection. most take a finish or semi finish and finish cut after roughing if tight tolerance, many consider <.001" a tight tolerance, where .001 to .005" i would say its a more normal tolerance.
.
4) many times a precision bore and keyways are +/-.0003" or less tolerance, thats when measuring taper is a bigger concern and often need a new sharp endmill for less taper. when recutting, tool deflection being less often it cuts more than expected
.
5) during tool change, tool runout can easily change if tool holder taper is dirty. obviously runout or wobble can effect dimensions
.
6) larger bores if parts gets hot the bore will get smaller when part cools off, and if cold coolant sometimes bore gets bigger when part back at room temperature. this is a common concern (temperature control) when doing tighter tolerances. some machines coolant is cold at beginning of work shift and coolant gets hotter during the work shift. also coolant evaporation can have a chilling effect especially when humidity is low. even if coolant system has a temperature control system to maintain +/-1 degree temp, evaporation chilling can be a problem with tighter tolerances and bigger parts
 
Have you asked him for help? Since he would have way more info than you've given us.

he was up in Michigan yesterday, overseeing the loading of a new mill we're getting, so he only had limited time and he's told me that if he wasn't available, to browse on here or ask for specific help. he's back now though, so we're getting it figured out.
 
he was up in Michigan yesterday, overseeing the loading of a new mill we're getting, so he only had limited time and he's told me that if he wasn't available, to browse on here or ask for specific help. he's back now though, so we're getting it figured out.

If you don't mind, please close the thread with a result. So often the search function turns up dead ends since the OP never comes back with the resolution.
 
he was up in Michigan yesterday, overseeing the loading of a new mill we're getting, so he only had limited time and he's told me that if he wasn't available, to browse on here or ask for specific help. he's back now though, so we're getting it figured out.

That makes sense, but for future reference, as Teachmeplease stated above if you have a question try to provide as much info as you can otherwise we're all just guessing.
 
.
1) usually end mills made for aluminum are sharper edge rake/clearance and work better than general purpose mills. its bad when end mill dull and aluminum sticks to cutting edge so bad you getting a hammer and screwdriver to knock buildup off
.
2) sometimes end mill corners get abrasive wear and bottom of bore is smaller. if you check bore with pin or plug gage and it starts in but doesnt go to bottom of bore, bore is tapered, same with checking keyways you check top to bottom looking for taper usually
.
3) when you double end mill stickout amount tool deflection increases 2x2x2 or 8x more. so if end mill stickout of tool holder amount changes it easily effects tool deflection. most take a finish or semi finish and finish cut after roughing if tight tolerance, many consider <.001" a tight tolerance, where .001 to .005" i would say its a more normal tolerance.
.
4) many times a precision bore and keyways are +/-.0003" or less tolerance, thats when measuring taper is a bigger concern and often need a new sharp endmill for less taper. when recutting, tool deflection being less often it cuts more than expected
.
5) during tool change, tool runout can easily change if tool holder taper is dirty. obviously runout or wobble can effect dimensions
.
6) larger bores if parts gets hot the bore will get smaller when part cools off, and if cold coolant sometimes bore gets bigger when part back at room temperature. this is a common concern (temperature control) when doing tighter tolerances. some machines coolant is cold at beginning of work shift and coolant gets hotter during the work shift. also coolant evaporation can have a chilling effect especially when humidity is low. even if coolant system has a temperature control system to maintain +/-1 degree temp, evaporation chilling can be a problem with tighter tolerances and bigger parts

Thanks tom, you covered about every bad situation that can happen, but somehow did not help the OP..?? :rolleyes5:
 








 
Back
Top