X offset for drills

[Vern Smith]

I usually always find the hard way to do anything and I'm sure this is no exception I probably missed it on the forums and could not find it in the Haas lathe manual but what is the easy way to set the X offset for drills, reamers, etc? I put an indicator in the spindle and indicated in the 1" bore in the tool holder but there must be an easier way.

An unrelated question, the machine blows air through the spindle for 5 minutes after the spindle stops. I can see a necessity to overcome the heat sink effect when the spindle stops but five minutes is a little long for the short duration low HP stuff I do. There has to be a parameter controlling this, does anyone happen to know it's number?

Vern

[Geof]

With the Offsets page open and the cursor on the tool you want hit F2 that should give it to you; it is stored somewhere in the Parameters.

Or at least it is in the SL10s; I wonder if the GT10 might not have it.

[Vern Smith]

Thanks Geof, I'll try that in the morning.

Vern

[HuFlungDung]

Vern,
Finding the offset that way should be okay....might be difficult, but you should be able to trust that position for that pocket until your crash something (but please don't ).

I don't have a Haas lathe, and neither do I have a tool eye on my lathe, but I've been working on streamlining some of my lathe setup so I can make short run parts with less fussing about. I've probably got a half dozen turning tools almost 'permanently installed' in the tool turret, so their offsets are good for any use, once they are set.

For drills and boring tools, I use a couple of Kennametal KM40 modular tool blocks, which are generally left in place in the tool turret. However, the offsets are all over the place whenever drills and/or bars are swapped. The nice thing about the Kennametal modular tooling, is that everything repeats very accurately when switching tools. This makes saving the offset information practical and useful.

So I've been working on saving this offset information, instead of just writing it down, I'm working on saving it in CAM. You can go to the OneCNC user forum and read my post about using G10 in the suggestions forum. G10 is used simply to load the offsets into the tool register, so if the G10 is within the body of your program, it is a facility to input values into the registers without screwing around with redundant measuring of tools that you've used once before.

I've gone from never using G10 before, to loving the usefulness of it, in only a week or two. Sure, it takes some careful record keeping to set up initially, but just think, whenever you finally crank out a good part, those hard-earned accurate offsets deserve to be saved.

As you will read in the user forum, you can actually save the offset data in the tool drawing, so it will be accessible from any new programs you create, plus you get to visually verify that the tool (which you should accurately draw a 3d model for) is actually the one that you thought it was

Maybe that is more than you wanted to know. But I hope by suggesting the idea, it might spark an idea or two in your mind, to reduce the fussing about of getting the lathe ready to make parts......

Having suggested that, I should also warn that using G10 for work offset and tool offsets is not without danger if you are a sloppy record keeper. Correct correspondence between the tools and their associated G10 offsets is essential.

I'm open to comments from other lathe programmers/machinists about doing this sort of thing. Theoretically it sounds good

[HuFlungDung]

One other thing I'll add about using G10. I have a preference for Kennametal Drill Fix insert drills. They are good for opening a hole at high speed, and they can also be used to enlarge the hole, as a boring bar. I always found it kind of a nuisance to deal with this kind of tool usage in CAM, because for drilling, you want the center of the drill to be the datum, but as soon as you begin using it as a boring bar, then you want the tip of the outermost insert to be the datum.

So with G10, it is possible to switch the datum by loading the change in the X offset right within the program, just prior to the particular usage one intends for the tool. This way, X0 will work for the drilling position, then as one bores the hole larger, the actual bore diameters can be programmed, as soon as the G10 switches the offset for that tool.

[Vern Smith]

Hu,

Good point, I adopted your G10 idea from the OneCNC forum for the mill over a year ago. The driving force then was my penchant for forgetting to change the diameter information in the machine tool register then programming compensation

I have not gotten far enough with the lathe program to set up the post for G10. I was not sure if the lathe program would take the tool library information and put it in a G10 line as the mill program does. I also have not found a place to put offset information into the OneCNC tool library. I was kind of disappointed that OneCNC lathe did not communicate with it's own materials library as the mill software does.

I've read the post on tool length offsets on this forum several times and am trying to incorporate both your and Geof's ideas. My current thinking is to make three plugs that can be inserted into my three available chucks that will all share a common distance from the spindle face. I will then set off all my tool offsets from these plugs. This way all the tools in the turret will share a common offset and adding a new tool will involve inserting the plug and setting up the new tool which will then share the common offset. I should insert a "I think" at this point because I don't know what I'm doing with zero experience.

My single half A'd effort yesterday says my three Haas supplied holders are within .003 in X, is this about normal? I know fixing X variations is easy to do with the tool adjustment register but what do you do about the variations in Y? Assuming there is such a thing as Y in a lathe

Almost all me project are very short runs so all the tricks to shorten set up time will be valuable to me. With an 8 tool turret the plug idea has a lot going for it if I can make it work.

I'm sure I will have many more uninformed questions after today's thrashing around.

Vern

[Geof]

Originally Posted by Vern Smith ...... I will then set off all my tool offsets from these plugs. This way all the tools in the turret will share a common offset and adding a new tool will involve inserting the plug and setting up the new tool which will then share the common offset. I should insert a "I think" at this point because I don't know what I'm doing with zero experience. My single half A'd effort yesterday says my three Haas supplied holders are within .003 in X, is this about normal? I know fixing X variations is easy to do with the tool adjustment register but what do you do about the variations in Y? Assuming there is such a thing as Y in a lathe ....Vern

Your 'plugs' will work; I just think it is overly complicated and using the end of the work piece is easier.

Regarding your 'Y' variation, which is really above/below center variation, you will probably find it as variable or more so, than the X. You can get really paranoid about getting the tool tip exactly on center but it is not really worth it. Only if you face across completely to the centerline will you ever see any effect of the tip being +/-0.005" above or below center.

[Vern Smith]

Geof,

I probably don't understand your system but if one uses the end of the work piece do you not have to reset all the tools (length) that will be used in the upcoming operation to the new workpiece as well? Will these tools not be set to a different length offset than the other tools that remain in the turret?

My concern with "Y" variations was for drills, taps, reamers, and such. I can see where a turning tool tip being a few thou high or low would not be a big problem, rigid tapping might be another matter.

Vern

[Geof]

You do understand, it is necessary to reset the tools for a new workpiece. As far as possible I leave basic tools in the turret and once the X offset is set I do not touch it (unless I change a tip making it necessary to tweak slightly}.

Z offsets I set for each job just by taking a facing cut with one tool and then touching all the others off against that face. Remember this is with a four place turret in a TL2 so very often I am changing tools between jobs and then I have to do both X and Z.

When you have more tools and are likely to leave them in place you approach of having a fixed reference point and then moving everything with the work offset is probably easier.

You are correct about off-center taps not being a good thing so it is worth finding the best holder and reserving it for taps. Incidentally you need to check the alingment with the spindle axis also because the Haas holders do have some slop when they bolt on and they can droop.

Drills it is hardly worth bothering about because all it means if the drill is going to rub on the lands and make a tapered hole which is likely going to be bored larger anyway.

Reamers you should be using a floating holder to accommodate small amounts of misalignment.

[Vern Smith]

Great, floating holders, another item to add to the growing needed tool list I plan on running the lathe with CAM programs and using a G54 and that's why I'm trying to establish common reference points.

I just ran into a little glitch that has me stopped dead in my tracks. The Haas lathe is halving all the X numbers my CAM program is outputting. I got suspicious when the manual instructs you to enter the measured diameter after hitting the measure X diameter button. A cursory search of the settings menu didn't show anything that could change this. I guess I will have to draw everything over sized in the CAM program. Maybe that's the way it's supposed to be done and they forgot to tell me.

Vern

[Geof]

Originally Posted by Vern Smith .....I just ran into a little glitch that has me stopped dead in my tracks. The Haas lathe is halving all the X numbers my CAM program is outputting..... Vern

This implies the CAM post is outputting radius measure not diameter; have you checked the post set up to see if it lets you choose between radius or diameter measure?

[Vern Smith]

Originally Posted by Geof This implies the CAM post is outputting radius measure not diameter; have you checked the post set up to see if it lets you choose between radius or diameter measure?

One of the moderators from the OneCNC forum got me straightened out. It's an election in the program's preferences but it defaults to radius and I was using the default setting. Now back to finding that floating tool holder