[joshetect]

maybe the problem was in your cam. Check your model, maybe you had a wrong height selected or an additional parameter in there from a previous op.

[IMT]

...The reason for running along the perimeter is to give a visual of where my machine limits are...

I have a 28x16 sub plate, I used the drag engraver to mark a rectangle at the machine limits. Then just stoned the burs. The oversize sub plate makes clamping large work pieces much easier.

[cobrakai]

Well here's the final product. I have a lot of very small parts that need to be held down with screws or tape, so the plate will turn into swiss cheese eventually. I do really like those fixture plates though, for clamping down larger work pieces.

[WOTDesigns]

just a thought: jog the z without a tool down as far as it was when you made that cut. Put an indicator off the table touching the nose. pull down on the head and see if you can get a thou or three of movement. These aren't insanely rigid machines. There is bow, flex and movement in the ball screws, gibs, base, and some thermal growth over time/temp. Add it all up and it can easily be 0.004" when indicating vs a 1" deep side cut. Your helix is pulling UP on the plate. Newtons law says it's pulling down on the head/ball screws/gibs as well. you likely lifted the table .001 and pulled the head down .002 and the spindle grew 0.001 = .004 (as an example). Even LIGHT cuts are not light cuts when there is a 1" DOC and a high helix EM pulling down on the head/up on the table. Just pointing out there are a million things that want to move. If you put the indicator on the head and touching the table and lift up on the table you will see 0.001+ movement. Mind you... I see movement when I do any of these on my Haas and Brother as well, less, but flex is ALWAYS there. Thermal growth is as well unless the entire machine is made of granite.

In the end there is a reason all controls usually have such easy offset adjustments... Program 0.005 HIGH and measure/inspect, adjust offset after seeing real world conditions applied to the cut and repeat the finish cut or program for a final finish cut. I do very tight tolerance work (+/-0.0005) all. day. every. day. There is only one way to hit those numbers and it's raking rough/finish/measure/finish again/measure/finish again. Even if I get it right at 8am it's wrong by 845 and needs the same process repeated over and over. 300+ parts a day and the same process on them all.

[RCaffin]

The reason for running along the perimeter is to give a visual of where my machine limits are.
I am not sure that you need to machine to the bottom surface of the plate for that?
Could you not machine to 1 mm above the bottom surface and leave it at that?
Or - evil thought, machine to 0.5 mm of the bottom surface and then grind/linish the tiny flange off by hand. Been there, done that too.

Cheers
Roger

[williamsmotower]

I would have put your plate on some parallels to get it off the table then cut the ends. I assume cutting the tends of your plate is purely cosmetic.

I use this trick all the time!

[mountaindew]

I see movement when I do any of these on my Haas and Brother as well, less, but flex is ALWAYS there. Thermal growth is as well unless the entire machine is made of granite.

In the end there is a reason all controls usually have such easy offset adjustments... Program 0.005 HIGH and measure/inspect, adjust offset after seeing real world conditions applied to the cut and repeat the finish cut or program for a final finish cut. I do very tight tolerance work (+/-0.0005) all. day. every. day. There is only one way to hit those numbers and it's raking rough/finish/measure/finish again/measure/finish again. Even if I get it right at 8am it's wrong by 845 and needs the same process repeated over and over. 300+ parts a day and the same process on them all.

Your setting up tool height offsets with electronic probes and touch plates on those machines Right? My experience with the Tormach system, measuring tool lengths on the bench with a plate and a height gauge does not always translate into real world precision when placed in the spindle and used. I mostly chase precision on the z axis. As long as I watch tool stick out / feeds speeds I rarely have x,y precision issues that I can measure anyway btw I get best results out of my Tormach when the shop is about 75 deg. Metal parts even fit and assemble better at that temp.

Anyway I was thinking after reading this post it might help to use a electronic tool height setter on the machine bed itself.
Thoughts?

[WOTDesigns]

Your setting up tool height offsets with electronic probes and touch plates on those machines Right? My experience with the Tormach system, measuring tool lengths on the bench with a plate and a height gauge does not always translate into real world precision when placed in the spindle and used. I mostly chase precision on the z axis. As long as I watch tool stick out / feeds speeds I rarely have x,y precision issues that I can measure anyway btw I get best results out of my Tormach when the shop is about 75 deg. Metal parts even fit and assemble better at that temp.

Anyway I was thinking after reading this post it might help to use a electronic tool height setter on the machine bed itself.
Thoughts?

I never bought into the offline measuring on my X3 nor Tormach. It takes seconds to measure on the machine and of all the places to save seconds, that's just not where I want to save them.

On my tormach I used an edge technologies 3" setter. On the Big Haas I got the probe and setter but it still didn't work well for my micro tools. I switched to using a cheap touch sensor that completes a circuit. More accurate that the Renishaw setter for those and takes me the same amount of time to touch off.

For the OM2A I had to add a wire to an alligator clip clamped to a small magnet. It has ceramic bearings so I have to throw the magnet on the tool holder body as I jog it down. I used the rolling pin method for months on the OM but this cheap Chinese sensor is more accurate after all. It did not fit on the fixture that I was using when I first started running this machine so I had to use the rolling pin.

The brother I bought with a Blum Pico setter for micro tooling "down to 0.005". So far that seems good but I won't start production on the Brother until tomorrow so time will tell. No probe on that one either since fixtures will sit for weeks at a time. Haimer was overkill honestly, but I love them and they are cheap.

I can touch off 7 tools in 2 minutes with those Chinese 'coolet circuit' probes and they are DAMN accurate. I'm talking 0.0001-0.0002 every single time. Those 2 minutes won't make or break my day.... But inaccurate tool LENGTHS would. I like measuring on the machine.

[GITERDUN]

I've got that terrible sinking feeling right about now.

I was making a new fixture plate for my mill. Basically it's a 1" thick piece of aluminum that is 1/4" narrower than the machine limits, so I cut at the X-Y limits using a 1/2" end mill. This provides a nice sacrificial work surface and also gives me a visual of my usable workspace.

Well I carefully measured my tool lengths, set the Z-zero on the table, checked the tram and ensured it was perfectly flat everywhere. Checked my tool length, tightness, collet tightness, everything. Brought it down to .0005" from the table and it just skimmed some sharpie from the surface. Perfect. I made my program bottom level .003" so that it would not get close, and leave a small amount of flash that I could remove with a razor blade. I took light depths of cut in a helical 2D-contour program to minimize tool deflection.

And yet... someway, somehow, the tool managed to cut into the table on the finishing level. Only about .001", but STILL! HOW DID THIS HAPPEN!? Yes, the groove is outside of the usable working area and shallow, but it's still a blemish on my table I managed to keep perfect for 6 years. After kicking myself for the last 3 hours, I am still confused as to how this happened. Could spindle/tool temperature cause a .004" growth in tool Z height? I now have a constant reminder for the future, but unless I know what happened it can happen again.


Now... even though I am 99.9% not going to do anything about it, is there a way to fix this? Could I remove the table and have that top surface ground flat in the future? Like I said, it's only about .001" deep.

It's a tool not the Mona Lisa. But if you are losing sleep, then just mill it deeper and fit a patch- you could even use brass and call it a customizing job.

[TurboStep]

...Only about .001", but STILL! HOW DID THIS HAPPEN!?

I can't tell from the photos but is this groove on both the left and right sides or just on the right?
Step

[tmarks11]

Now... even though I am 99.9% not going to do anything about it, is there a way to fix this? Could I remove the table and have that top surface ground flat in the future? Like I said, it's only about .001" deep

Yes, you can get the table ground on a large surface grinder, probably cost you $200-300. No fears, they can make it flat and beautiful again. I wouldn't bother, though, since based on the location, it probably won't have much of an impact on future machining.

I never bought into the offline measuring on my X3 nor Tormach. It takes seconds to measure on the machine..,

+++1. Never really got the whole "offline tooling measurement" concept, since it is so quick to do it directly on the machine, and is more likely to be accurate.

[mountaindew]

+++1. Never really got the whole "offline tooling measurement" concept, since it is so quick to do it directly on the machine, and is more likely to be accurate.

This is what I was thinking. Measuring the tool offset with the machine itself could add that little precision that I seem to miss at times using 2 different tools to get the numbers.

[IMT]

I have found Tormach's offline setup to be repeatable to +/- .001, when I need better I use my tool setter on the machine. Also use the tool setter for non-TTS tools, 3/4" EMs directly in the R8 collet.

[RCaffin]

Never really got the whole "offline tooling measurement" concept, since it is so quick to do it directly on the machine, and is more likely to be accurate.
Now try doing it on the machine when you are running high speed production with an ATC with 12 different cutters.
Yes, you need high quality spindle mounts and (say) matching BT30 or BT40 holders.
Not going to happen with R8

Cheers
Roger

[tmarks11]

Now try doing it on the machine when you are running high speed production with an ATC with 12 different cutters

Yes, I get where it makes sense in a production setting with a high speed cnc mill and a limitless belt of tools. Offline is the way to go (but not the amateurish offline setup Tormach sells).

But on a slow speed mill like Tormach with only an 8 tool toolchanger?

[RCaffin]

Don't have a Tormach, so I'll hand that one off to someone else.
(I use ER25 collets, but I hand-code as well.)

Cheers
Roger

[cobrakai]

Hey guys,
Following up on this thread with further frustration. I haven't damaged my machine any further, but I am currently working on a project that requires .001" precision in the Z. It's some thin 4130 sheet and I'm going at it entirely with a 1/8" 4fl cutter.

I went to great lengths to set my zero at the aluminum work surface, and then in CAM I only go to .003 above the surface. I know, I made this mistake before resulting in cutting my table, but I'm less concerned about the aluminum surface plate as making it all the way through without a burr is more important. Anyway... the program is pretty long due to all the small features. The machine runs for almost 2 hours at 3000RPM. No tool changes, coolant flow the entire time. By the time the machine is taking the final Z .003 perimeter cut, it is now touching the surface plate and leaving a mark. I would say a reasonable estimate is that my Z is dropping .0035" from the start of my job to the end. Is this normal!? It seems excessive to me.

I have .0010 to .0012" of backlash in the Z, which is normal according to Tormach (I jog down with an indicator to a set point, and it takes .001" of upward movement before it starts moving up). The temperature of everything when I start is around 55-60 degrees, and the spindle is warm to the touch when it's done, I'm gonna say about 100 degrees.

It just seems excessive and hard to make super accurate parts. Are there any things I can check to confirm this? What about some process suggestions to deal with this variation from beginning to end? I guess the first thing I should do is figure out where the movement is coming from, and if it goes back to where I started by the time it cools down overnight.

[RCaffin]

Just a thought: is it possible that the 50 degree rise in temp is causing that movement (0.0035") of the tip of the cutter from thermal expansion? I can readily imagine that happening.

Cheers
Roger

[cobrakai]

I guess if I have a total stickout from the spindle head of 3 inches (tool holder and tool), a rise in 50 degrees equals .0034". It could really be that simple huh?
https://www.engineeringtoolbox.com/l...on-d_1379.html

How do the pros deal with this? Run the machine for an hour, set the zero, then run the job?

[RCaffin]

It might be a little more thanjust 3" as the real reference point is the ball-nut on the Z-axis lead screw. But part of that framework might not be so hot. Interesting that the figures come out so well.

How to handle it? Water-cooled spindle, mostly. And occasional reset of zero.

Cheers
Roger