[inov8r]

I am using a PCNC 770. I use it for light engraving of small pockets. My Z backlash is .0009, up and down. This tells me that the gib is tight enough to hold the weight of the headstock. I am suspecting that I am experiencing some creep during the dozens of up and downs of engraving and am getting poor depth results. I am wondering if I were to loosen the gib to the point that the weight of the headstock allowed the z axis to always run on the bottom race of the ballscrew, would this leave the headstock way floppy loose and cause problems not obvious to me? I am thinking that the super light cuts I make would not have much of a lateral effect on the spindle. But I wanted to throw it out here in case someone has done this and has any pointers or warnings.

[JohnToner]

Try it on some scrap and see what happens.

[Steve Seebold]

If you have to hold depth tolerances of tighter than + or - .001, I suspect you bought the wrong machine. My PCNC 1100 will hold + or - .001 all day long.

[inov8r]

If you have to hold depth tolerances of tighter than + or - .001, I suspect you bought the wrong machine. My PCNC 1100 will hold + or - .001 all day long.

So because your machine won't, nobody else should try and they bought the wrong machine! Interesting point of view.

[tmarks11]

I am using a PCNC 770. I use it for light engraving of small pockets. My Z backlash is .0009, up and down... I am wondering if I were to loosen the gib ...

I don't really understand how that would improve your situation; I think it would make it worse. Allowing the head to shift would tend to make the cutter dig in at on an edge as it torques the head, giving you a worse surface finish.

Maybe if you gave us all some more details.

Material
DOC
Speed & feed
Type of cutter

Do you have a measurable change in DOC, or just poor surface finish?

[Ken_Shea]

Does this backlash show up throught the full length of Z or just where you'be been using is a lot?

Thinking maybe you could position the stock at a higher plane to get reif of the issue.

Ken

[jid2]

Your spindle can grow with heat, and see changes of .001". Try warming up your spindle before you set your Z height and see if that helps.

[Steve Seebold]

So because your machine won't, nobody else should try and they bought the wrong machine! Interesting point of view.

No, that's not what I am saying. I just don't want to work that close any more. Actually, if I get a job that's closer than +/-.005 I'll usually turn it down.

I just picked up a 25 piece job that has +/-.005 all over it. It's gonna be fun.

Most folks don't have tools to check +/-.001 anyway. You can't consistently measure within .001 with a dial caliper, and there is absolutely no way you can accurately measure the inside of a hole with a caliper unless you do some math.

[inov8r]

I don't really understand how that would improve your situation; I think it would make it worse. Allowing the head to shift would tend to make the cutter dig in at on an edge as it torques the head, giving you a worse surface finish.
Maybe if you gave us all some more details.

Material
DOC
Speed & feed
Type of cutter

Do you have a measurable change in DOC, or just poor surface finish?

My thought was that you should be able to loosen the gib to the point that the weight of the head would allow it to slide freely without giving up any appreciable accuracy. There is not alot of torque applied to a .005" cutter at 10 to 20K rpms, so that isn't going to me much of a issue. The fact is that I am trying to solve a depth issue on this machine and I am looking to incrementally remove the variables.

[inov8r]

Your spindle can grow with heat, and see changes of .001". Try warming up your spindle before you set your Z height and see if that helps.

I thought of that, soI put an indicator on it when it was warm and let it cool and there was no appreciable shrink

[inov8r]

Does this backlash show up throught the full length of Z or just where you'be been using is a lot?

Thinking maybe you could position the stock at a higher plane to get reif of the issue.

Ken

The backlash is acceptable, I would just like to be able to work around it as much as I can. Like I said I am seeing some depth inconsistency and I am trying to assess the problem one issue at a time.

[tmarks11]

Most folks don't have tools to check +/-.001 anyway. You can't consistently measure within .001 with a dial caliper, and there is absolutely no way you can accurately measure the inside of a hole with a caliper unless you do some math.

Which is why you use a micrometer and a telescoping hole gage. A granite surface plate, a height gage, a set of gage blocks, and a 0-4-0 DTI also allow measurements in the tenths range without too much work.

Not too hard to get tenths accuracy in measurement. All things that should be in your toolbox.

Some day I will stumble across a set of hole micrometers on craigslist and I can throw the telescoping gage in the bottom drawer. I don't like them, but not to the tune of dropping $600++.

[Steve Seebold]

Which is why you use a micrometer and a telescoping hole gage. A granite surface plate, a height gage, a set of gage blocks, and a 0-4-0 DTI also allow measurements in the tenths range without too much work.

Not too hard to get tenths accuracy in measurement. All things that should be in your toolbox.

Some day I will stumble across a set of hole micrometers on craigslist and I can throw the telescoping gage in the bottom drawer. I don't like them, but not to the tune of dropping $600++.

Check with Shars. They have a .2 to 1.2 inside mic for $41.95, 1-2 for $50.95, 2-3 for $69.95 and a 4-3 for $79.95.

I have 3 inside mics ranging from .2 to 3.0. and I have less than $100.00 in them, but I bought them about 10 years ago. Yes, they are Chinese, but for what I do with them, they work just fine.

[tmarks11]

Check with Shars. They have a .2 to 1.2 inside mic for $41.95, 1-2 for $50.95, 2-3 for $69.95 and a 4-3 for $79.95.

Thanks, I will give those a try. They gotta be better than me with a telescoping hole gage and a mic. I worked long and hard to get a good feel for the process, but if I haven't touched them for 6 months, I lose the feel.

I would like a set of internal 3 pt hole micrometers, but that is way done the list of "wants", not even close to the "must have" category.

[inov8r]

Your spindle can grow with heat, and see changes of .001". Try warming up your spindle before you set your Z height and see if that helps.

Here is a little update on some testing I have been doing. The pic is of a series of cuts to help me find some depth inconsistency I have been having. You can't see in very well in the pic but I started with a square in the center that was set to cut .0001", this would let me know if I was zeroed correctly. And it scratched the surface perfectly. The circles and moon shaped cuts in each set were all cut to the same depth and overlap so I could see any major depth issues within a set (none found.) The top set is cut .001" and ended up a little under. The second set was cut .002" (2 passes @ .001") and ended up slightly under. Set 3 cut .003" (3 passes @ .001") and ends up a few tenths over. Set 4 cut .004" (4 passes @ .001" ) and ends up a few tenths over .005". Set 5 cut .005" (5 passes @ .001") and ends up .0075". Set 6 cut .005" (1 cut @ .005") also ends up .0075.

The logical conclusion was to recheck for an expanding spindle. I'm not sure what I was doing so wrong before but I put an indicator on and let it run till it warmed up nicely and low and behold it grew over .002"!! I am using the speeder and I suspect the aluminum housing has a lot to do with this much expansion.

[CadRhino]

I was watching an NYCNC video and he was warming up his spindle. This must be why. Thanks for sharing.

Here is a little update on some testing I have been doing. The pic is of a series of cuts to help me find some depth inconsistency I have been having. You can't see in very well in the pic but I started with a square in the center that was set to cut .0001", this would let me know if I was zeroed correctly. And it scratched the surface perfectly. The circles and moon shaped cuts in each set were all cut to the same depth and overlap so I could see any major depth issues within a set (none found.) The top set is cut .001" and ended up a little under. The second set was cut .002" (2 passes @ .001") and ended up slightly under. Set 3 cut .003" (3 passes @ .001") and ends up a few tenths over. Set 4 cut .004" (4 passes @ .001" ) and ends up a few tenths over .005". Set 5 cut .005" (5 passes @ .001") and ends up .0075". Set 6 cut .005" (1 cut @ .005") also ends up .0075.

The logical conclusion was to recheck for an expanding spindle. I'm not sure what I was doing so wrong before but I put an indicator on and let it run till it warmed up nicely and low and behold it grew over .002"!! I am using the speeder and I suspect the aluminum housing has a lot to do with this much expansion.

[jid2]

Great test. Thermal growth in the Z axis related to the spindle is an issue most machines face. Even machines with big price tags confront it. Most people mitigate with a proper spindle warm up cycle. When .002" is 50% to 100% of the feature size, like with engraving it's critical. Many people also probe to get a perfect zero on the surface to be engraved.

[EvolveES]

I wanted to add that with careful adjustment you could probably get the Z backlash better than 0.0009" we currently have just a little over 0.0001 bcklash in the X and Y and the Z (which we have never adjusted yet because i don't want to climb all over the machine) is currently at 0.0004". You can adjust the jibs and also the bearing preload to reduce the backlash (this assumes that the ball screws are installed well). It doesn't seem like it's an issue for you so you may not be interested but if any of the back lash get over 0.0005 i start trying to make them better and have had good luck doing it. I hope you can get the thermal issue under control