What's new
What's new

Hole interpolation accuracy with endmill

cgrim3

Cast Iron
Joined
Dec 4, 2020
Location
Baltimore
Listen, I am sure this has been covered a number of times in different threads, but I wanted to ask the question. We interpolated a 1.002" hole with a .5" diameter 2" loc garr endmill in aluminum. The machine is a 2007 daewoo 3016 with cat 40 taper and fanuc Oi-mb controller. We used a bore gauge to check the diameter of the hole. The hole size tolerance is -0 +.001. The machine had no problem holding that size, but the hole size variation from interpolation is about .00035 to .0004. I assume this could be from a number of things. Possible endmill/toolholder runout, endmill deflection since it is a 2" loc, and/or backlash. If this variation is all from backlash, is .00035-.0004 acceptable or should I try to get it closer?

If I can account for the backlash in the controller, how do I do that? Or is it even needed if .00035 is close enough?

Thanks,

Chris
 
Sooo many variables.

What are you speeds/feeds? More importantly, what are your look ahead / shape comp settings?

Sure, backlash can be comped out, but an out-of-round hole doesn't tell you anything about backlash. A lost motion check is really easy to do, and will tell you a lot more.

Let's start by looking at your process, and then go from there.
 
we are using smoothing and feed optimization. We are using fusion 360. The tolerance set for smoothing is .00001

Feeds and speeds: 2000 rpm, feedrate of 10 ipm. It is aluminum and we could have gone faster. The machine has an 8000rpm spindle so we try not to go too fast. This is a one-off part so we didn't apply super super fast feed rates for production.

I do not know how to apply look ahead in fusion or on the machine. How do you do this?
 
The hole does fall between the min and max. Nothing wrong with the hole. It is within tolerance. I was just reading on here where people are saying they can get their interpolated hole sizes within .00001 - .00005. That's insane. To do that, would you have to replace your ball screws, bearings, and fine tune the controller for backlash? I mean our machine is from 2007.

Chris
 
I do not know how to apply look ahead in fusion or on the machine. How do you do this?

It varies by builder. I recommend that you investigate this. Fusion dumping out path at a resolution of .0001in won't mean anything if your controller is defaulting to .005in shape compensation.

Typically on a Fanuc you are looking for G08 or G05.1 to turn on basic lookahead. Often the builder will also provide auxiliary codes for fine tuning.
 
I was just reading on here where people are saying they can get their interpolated hole sizes within .00001 - .00005. That's insane.

I can easily comp an interpolated hole by .0001in increments on our DMG MORI, and can check with a deltronics pin accordingly.
However, checking with a pin does not actually verify the form of the hole. I can guarantee that when I interpolate a hole to within .0001in diameter (and it passes a check with pins) that the hole is not round within .0001in. The pin check (and usually the customer) won't notice if it's a little oblong.

Having a tight machine is critical, but a tight machine doesn't help anything unless your process control is actually good enough to achieve repeatable and measurable results.

All that said - you can get a ballbar test done on the machine. That is basically the ultimate test of it's ability to travel in an accurate circle. Ballbar tests are often publicized for the best machines on the market. There are very few machines in the world that can interpolate a circle within .00001 to .00005, and that's before we even consider process variability.
 
A lot is going to depend on the control as well as the machine but often G05.1 Q1 is simple HPCC smooth interpolation mode (which turns short lines into arcs) and G5.1 P1 is multibuffer which is lookahead. Pretty sure this is FS15 format

Moving at 10 IPM and having an actual arc as a toolpath I doubt you will see any difference with high speed codes
 
The hole does fall between the min and max. Nothing wrong with the hole. It is within tolerance. I was just reading on here where people are saying they can get their interpolated hole sizes within .00001 - .00005. That's insane. To do that, would you have to replace your ball screws, bearings, and fine tune the controller for backlash? I mean our machine is from 2007.

Chris

I highly doubt that, 0.0001-0.00005 yes
 
Throw it across a CMM and you start to learn that nothing is really round or cylindrical LOL.

Something that I just need to hold a 0.001" tolerance zone? I would probably helical bore / interpolate for one-off or short run but I'd bore or ream for anything more than a handful of parts. I have found that the surface finish isn't as good helical boring but it seems to take up some of the slop by averaging it out as it goes around in a circle several times.

Once you get to sub-thousandth for cylindricity call I'm going to be boring or reaming for sure.

But I'm not exactly an experienced machinist so take that FWIW.
 
The hole does fall between the min and max. Nothing wrong with the hole. It is within tolerance. I was just reading on here where people are saying they can get their interpolated hole sizes within .00001 - .00005. That's insane. To do that, would you have to replace your ball screws, bearings, and fine tune the controller for backlash? I mean our machine is from 2007.

Chris

"Threading the needle is a task for the young." I have a five year old machine that's only ever been used by me, for prototypes and short runs, and that gets a laser and ballbar calibration every year. On a 14 year old machine, yeah, especially if it's been run at or near capacity, I think you'd need a rebuild to get that accuracy back.
 
Most* of the people boldly proclaiming very small numbers on interpolated bores don't have the experience or the measuring equipment to back it up.

Pretty easy interpolate a hole on size with a tight tolerance just measuring the diameter with a bore mic, gauge, or pins. Most interpolated bores are not round, not cylindrical, not straight, but you need more sophisticated equipment or techniques to recognise such.

Like Rick said, put your perfectly interpolated hole on a CMM or Talyrond and get a nice reality shock.

People frequently recommend helical interpolation to get better holes, but that only addresses taper.

There is no substitute for single point boring when you need holes that you can count on.

FWIW, a good way to remove steps due to lost motion, or lobing from imperfect motion control, from an interpolated bore/boss or profile is to do an additional finish pass in the opposite direction. Climb mill first, then conventional. I guess doing this in combination with helical would be about the best you could ever hope to achieve by interpolation.

*Obviously there are exceptions, no need to get mad if you're one of those who know what you're doing.
 
The ratio of cutter size to hole size plays a part as well. Skim a 1" hole with a 1/8" endmill, and you'll see every imperfection of the machine's movement show up on the hole wall. Cut a 1/2" hole with a 3/8" endmill, and any errors will be minimized.
 








 
Back
Top