Boring Brother Questions (also

Have a job I need to get finished up for a customer. Customer used to make these in house, but looking to outsource this type of work to me. For simplicity sake, all we are concerned about is one hole and the accuracy of that hole. Customer always bored these holes using a boring head, for accuracy. Hole is for a sliding component in a piece of tooling.

I want to start a whole other thread with questions concerning "High Accuracy Mode" as I am starting to run into minor accuracy issues that I didn't think I would need to call out a mode, but I think it does play into this topic a little, looking for input and suggestions.

Hole is ~.500 (changes from tool to tool) the land where the tool slides is also about 1/2" thick, again, varies depending on the tool. The customer used to setup the block, again, which varies 2-3" thick, bore the hole all the way through, then flip and machine the backside. I am looking at machining the backside, flipping, then milling the top side. However I am hesitant as to the resulting accuracy from milling the hole instead of boring.

Using a High Accuracy Mode, does anyone here have experience machining a precision hole on their Brother, and what kind of accuracy did you get as a result?

In regards to boring, what are you using as a boring head? I had two different tooling reps look up holders for my Criterion boring head, they have been discontinued, or are (in my opinion) crazy expensive. (One quote I got back was $400+)

I have seen videos of machines boring, what are they using? What are you using?

thanks for the input.

Good boring heads aren't cheap, $1500 or more.
High accuracy can only do so much, but you can make it more accurate by slowing your feedrate down as well.
How fast is your feed in the 1/2" hole?
And how deep is the hole?

I would drill, interpolate, and ream. Really need to know tolerance, material, and size. You might be able to just interpolate. Practice with scrap first, of course. If you interpolate, dedicate one tool to do the finishing. Worst case, you might have to run the hole undersized, and adjust cutter comp to get it to perfect.
If you are running into other accuracy issues, explain what's going on. Could be technique or cutter issues - I always like to blame the machine last.
good luck!

What kind of holder do you need? Just looked and Lyndex no longer has them, bummer.

Thanks for all the quick replies guys! Will include a bit more info to try and clear things up.

Mtndew said:

Good boring heads aren't cheap, $1500 or more.
High accuracy can only do so much, but you can make it more accurate by slowing your feedrate down as well.
How fast is your feed in the 1/2" hole?
And how deep is the hole?

Click to expand...

I know good boring heads cost money, and I know my Criterion isn't a Wohlhaupter, but it has served me well, and I was hoping to continue using it until someday I have the cash or job, to buy a really nice one.
I am setting up a test piece right now, I was either going to use a 1/4" 4FL 3437 rpm 22 ipm or potentially a YG 6FL 8 or 6mm. They are great finishers with tool steel, haven't set one up yet for feed/speeds.

eaglemike said:

I would drill, interpolate, and ream. Really need to know tolerance, material, and size. You might be able to just interpolate. Practice with scrap first, of course. If you interpolate, dedicate one tool to do the finishing. Worst case, you might have to run the hole undersized, and adjust cutter comp to get it to perfect.
If you are running into other accuracy issues, explain what's going on. Could be technique or cutter issues - I always like to blame the machine last.
good luck!

Click to expand...

Tolerance... this is a small point of irritation. It would take too long to explain in depth, suffice to say the accuracy is important enough that I have concerns whether interpolating would generate the circularity/cylindricity (?) adequate enough for the tool. Material changes from tool to tool, A2, D2, D6, A11, CPM-10V, and one other I am forgetting about...
Size also varies, thickness of the tool, diameter of the hole, thickness of the working area, etc.
Setting up a test piece right now. Normally I would agree with you, but with this parts family, the hole diameter changes, frequently. None are "standard" diameters. Each would require a custom reamer. They repeat... once or twice a year. Some every couple years. Just not worth having custom tooling made. Another reason I was hoping to interpolate them.
I'll get more involved with the accuracy issues in another thread. There are a lot of variables, and this is a new machine for me. "What we have here, is a failure to communicate!" I know the machine is capable of better accuracy than me, I know what I want, I just need to know how to set it and communicate with the machine.

DavidScott said:

What kind of holder do you need? Just looked and Lyndex no longer has them, bummer.

Click to expand...

The Criterion is a 7/8-20 thread if I remember correctly. B30BH-0875-1.75 was the part number I was given.

I have a 1/2" straight shank for it, and can stick it in a endmill holder or collet holder, but I really don't like holding boring heads that way. Now, if someone made a Moore to BT30 holder, I would be all set, I have 4 or 5 REALLY nice boring heads for my Moore

FWIW, I used to take a .498" endmill and interpolate a .500" hole with it, on a Haas. Great fit using regular minus (+0/-.0002") gage pins. Was it round? Dunno, was it great for what I was doing, YES!

IIRC it was only 2x diameter, obviously the greater the length of your endmill the bigger the problems with fit/taper/finish, etc...

edit: Criterion is bottom of the barrel IMO for a cnc, if you do need to bore them, good a 'good' set with tenth setting. I have used these and they are pretty awesome for the price ($1500 set?) (switched to a high positive rake insert for alum)

Techniks BohrSTAR 43 Triangular Insert Boring Kit – Range .314" up to 1.962"

I have a few Lyndex BT30 7/8-20 holders but no extras, sorry. I would hope someone still makes them. Sure Criterion is not the best but it does the job if you only need to bore a few holes every few years, and you have one.

This is definitely not a high accuracy mode question. you will be programming a couple of inches per minute if you interpolate this. HA mode comes into play when you are programming much faster say in aluminum at 100 IPM plus. The issue I see is the length to diameter ratio for your cut. You may be able to leave about .oo5" for the finish pass, take something like a 7/16 neck style end mill and helical interpolate the bore moving Z down as it interpolated. When machining IDs like this with an end mill that is close to the size of the bore the feed rate becomes minuscule. There is a formula to compensate for this. ((Dwork - Dcutter)/ D work) x theoretical feedrate. For example, if you normally would cut this material at 20 IPM in a straight line, to get the same chip load in the ID bore it will be ((.5 - .437)/.5 x 20 = 2.52 IPM This is crucial! HA mode is not necessary at 2.5 IPM! The Brother will interpolate a very round bore.

Ran a test piece just to experiment.

Material was a little scrap of most likely 1018/1045. Diameter of the hole is .464, depth of hole for this one is .450 (through hole, this diameter is only .450 deep)

1/4" 4FL 3437rpm 2.750 ipm helical boring with the endmill with .01" pitch

I don't have a CMM or anything fancy to check circularity of the diameter other than to put an indicator in the spindle and run it around. Using a .01mm Interapid, if I zero at 12 oclock I get; -.005mm at 3 oclock, -.01mm at 6 oclock, 0 at 9 oclock. This is at a depth of around .075"

I may drop this off at a friends who does have access to some fancy toys and see what he gets for results.

If I probe the bore, at about the same depth I get .4630, and it shifts my work coordinate plus .0001" in X and -.0001" in Y.

All the time I have to play today!

Frank, thanks so much for your input, will try some better experimentation with a some different combinations tomorrow or saturday.

Did you not mention the tolerance requirements because there are several tolerance callouts for the bore and they change a lot between pieces? Like Diameter, Roundness, Concentricity top-to-bottom? Really needs to be a tolerance to determine what works and what doesn't, right?

Can this hole be honed? Sunnen makes some really neat tooling, but if $400 is high it might be out of your budget.

Im willing to bet you can bore a better cylinder than you can interpolate, problem with boring in CNC's is the tool change, that directly governs how well you really get to hold size part to part.

If your Criterion boring head is just a std one that takes boring bars, no need to buy custom tooling, just cut down a CCMT lathe bar of the correct dia and add a sleeve if needed to take up the slack in the head. I find then using a CCGT sharp style insert i can hold better than 10 microns on hole diameter part to part with no tool changes. Thats as good as i can measure bores reliably, with the new spindle bearings im pretty dang confident there round to single digit microns too and thats on way less machine than your getting to use. Using the sharp CCGT inserts even in bores more than 2" deep i can not measure any taper either from measurement or feel of precision ground parts sliding on through. Sharp tool small cuts and thats low forces hence low deflection.

Fal Grunt said:

Material was a little scrap of most likely 1018/1045. Diameter of the hole is .464, depth of hole for this one is .450 (through hole, this diameter is only .450 deep)

1/4" 4FL 3437rpm 2.750 ipm helical boring with the endmill with .01" pitch

Click to expand...

Why are you helical boring this with an end mill?
Why not just circle interpolate?

Just to clarify, this is one part. One and done. I might make another one in 6 months or 3 years. Depends on how fast the customer wears out the tool. There are many similar parts in the part family, but they are all different. They all run different quantities and time frames. I can count the number of holes I bored last year on both hands... if I pick up all their work, making these parts, it might be one a month.

DethloffMfg said:

Did you not mention the tolerance requirements because there are several tolerance callouts for the bore and they change a lot between pieces? Like Diameter, Roundness, Concentricity top-to-bottom? Really needs to be a tolerance to determine what works and what doesn't, right?

Click to expand...

Sure the tolerance is important, and typically that is what dictates process, but I did not mention it for several reasons. Primary being I did want the thread to degenerate into a pissing match about customers and tolerances, which I have seen happen many times here on PM.

Red James said:

Can this hole be honed? Sunnen makes some really neat tooling, but if $400 is high it might be out of your budget.

Click to expand...

I almost bought a Sunnen Hone (the floor machine) last year. Guy wanted $500 for it, it was pretty rough, I offered him $300. He turned me down. About 6 months later I found out two details that really upset me. He wound up selling it for $300 to someone else, and it had a cabinet full of stones that he never mentioned or showed me when I looked at the machine.

$400 for a holder to mount my boring head is expensive, but buying a hone is something that has been on my list for awhile and might be something I look at.

adama said:

Im willing to bet you can bore a better cylinder than you can interpolate, problem with boring in CNC's is the tool change, that directly governs how well you really get to hold size part to part.

If your Criterion boring head is just a std one that takes boring bars, no need to buy custom tooling, just cut down a CCMT lathe bar of the correct dia and add a sleeve if needed to take up the slack in the head. I find then using a CCGT sharp style insert i can hold better than 10 microns on hole diameter part to part with no tool changes. Thats as good as i can measure bores reliably, with the new spindle bearings im pretty dang confident there round to single digit microns too and thats on way less machine than your getting to use. Using the sharp CCGT inserts even in bores more than 2" deep i can not measure any taper either from measurement or feel of precision ground parts sliding on through. Sharp tool small cuts and thats low forces hence low deflection.

Click to expand...

I hadn't even thought about the tool change, in the past when boring, we always hand loaded the boring head, but again, I have little to no experience with production. If we used the boring head, it was loaded, bored out the holes that needed bored, then we moved on to the next part.
I am confident that the machine will bore the holes accurately enough, I just can't seem to find a boring head & holder for the BT30 without using a straight shank or buying a whole new "kit". I might wind up saving up and buying Mari-tools kit?

Mtndew said:

Why are you helical boring this with an end mill?
Why not just circle interpolate?

Click to expand...

I initially did circle interpolate, then Frank recommended helical boring, so I gave it a try. Helical boring did seem to reduce the taper a few tenths.

This morning I had a few minutes so I indicated around the bore and got it as close to zero as I could. What I found promising, is the bore seems to be round within a tenth or maybe two. What I found odd was the position of my zero moved?


Sorry, looks like PM mixed up the pictures

Part was ran on G54, then I indicated the hole in and set to G55.

Mtndew said:

Why are you helical boring this with an end mill?
Why not just circle interpolate?

Click to expand...

^^^^^ this.
No need to helical. End mill can helical cut, but they don't work best that way in my experience, especially if you are trying to finish a hole to size. If I had to do a hole that way, I'd semi-finish, and come back with an end mill that I used only to finish the hole, just circular interpolate, optimize speed and feel. If possible, don't use the bottom corner of the end mill. I know you have to if it's a blind bore, etc, but I never (here YMMV) want to cut with the corner unless it's required and designed for that. If it's dropped, bumped on the bench, anything like that will affect the corner right? Sorry if you know that (likely do) but others will come along here and read this at some point that don't.

I did not find this thread about machining on a Brother boring at all.

And do 2 passes at the same time so there is no trace of where you entered the profile, with the largest radius lead in and out you can achieve.

A necked down EM can help with taper while helixing a deep hole.

BT30 Cheap but usable criterion style shanks are on the bay, sure there not brand name, but then run out does not matter with a single point tool like it does with a end mill.

yeah Franks Kit is sure a nicer option if you want to splash the cash that much, it certainly is the kinda thing that's useful to have kicking around for future jobs too.

Tool change did cause us issues on a tight bearing bore but that was on a nearly as in sub a couple of year old Haas. That was tool changer loaded though.

That would bring the question, does positional accuracy matter as much as bore accuracy? Can the bore be very precise but be .0005” shifted in relation to the edge of the part?