Dumb setup question

[holedpiston]

Got a VMC15 here with 88HS control running format 2 on code generated by CamWorks. Everything works great if I set tool heights to part zero and use zero for the fixture Z. Today I tried setting tool heights to the table and putting the part origin height in for the fixture Z value.

Initially, what happened is I would get Z axis overtravel during a tool change. To fix this I tried adding E0 to the line just before the toolchange. This worked to prevent the Z overtravel, but I also got an unsettling XY shift as the head retracted. Also, at the end of the program when the table normally comes to the full +Y home position, I got an overtravel fault there, too.

My post outputs this prior to a toolchange:

Z0 H0 M05, which I tried changing to Z0 H0 E0 M05

End of program typically looks like this:

Z0 H0 M05
X0 Y0 E0
M02

Not sure which part of that sends the table home.

Anyway, can anyone lift my cloud of ignorance here as to what is going on? I would really like to continue setting tool heights to a non job-specific reference for obvious reasons.

Cheers

[fpworks]

Like you, I always input a 'z' value on my fixture/workpiece offsets, so the tools are not dependent on the setup.

The only thing I have before a toolchange command is M5.

The M6 command automatically (and simultaneously) cancels your tool length offset and the 'z' value of your current work offset, so the only time it isn't safe is if your workpiece is REALLY tall and your tool can hit your setup when at the tool change position.

At the end of my program, I bring the table to max y+ also, but I use the following line in my cam post to do so:

G0 X0Y0Z0 E47 H0
Where E47 is usually X0 Y8. Z0 I say "usually" because if a setup is offset on the table (in x) I just go into the offsets and put X-10. or something like that in E47.

If you were wondering why I don't use E48, that is my location of my electronic tool length touch probe.

If I haven't covered it here, please "post" a sample post, as well as the values in your tool length offset and fixture offset.

Justin

[fpworks]

Sorry, should have read your post more carefully.

"Z0 H0 M05" can cause a z axis overtravel because the z component of your fixture offset has not been cancelled.

Here is how I execute a tool change

G1, G0, etc... (cutting away)
M5 (this kills the spindle and cancels M7 and M8)
T2M6

You said the following code give you problems:
Z0 H0 M05
X0 Y0 E0
M02

The first line cancels your tool length offset, but not your workpiece offset, so this is how you can get z axis overtravel.

The second line return the table to the home position, but not the spindle.

[holedpiston]

Thanks for the insights. I think I just need to experiment a little and then edit my post.

Cheers,
Keith

[perrettamachine]

I don't preset tool lengths on the Fadals in my shop. We change out jobs every couple of days on them, and just take a couple of minutes of setup time to set each tool to to the programmed z zero setting. The tool setting cycle in the controls makes it very simple.
I haven't been convinced to do otherwise. Maybe someone can give me a good reason to change. The fact that I don't have enough tool holders to designate for the variety of tools I use may be one reason.
I end my programs like this:
N61G53Z0
N62X0Y0Z0E0H0
N62.1M6T1
N63M30
I let the operator put whatever value he wants to change parts in the x and y location on N62. I call up my first tool before the progaram ends.
I use fixture offsets all the time, but usually just in the x and y axis.

[holedpiston]

If I had a touch probe, I probably wouldn't be worrying about this, but I change setups many time per day. The tool setting cycle in the control is good, but it gets tedious after the Nth time. I try to keep track of all the tool settings in my head between setups and just modify them without actually touching off. Sometimes I get it wrong with predictable results.

[timf]

i use an offline tool setter for every tlo i get.

most of my tables have multiple jobs/operations set up.
even if it is a new job i like to cycle thru all ops before i commit to the first.
the really cool thing about the preset tlos is any tool in my rack is usable on any operation.

since the tlos are from the spindle nothing changes from set up to set up for the tool.
with the z number in my fixture i can use the same spot drill or endmill in any operation, even swap tools between machines.
alot of times the second or third op will have the same tools so i just program them with the same tool numbers when writing the code and the operator only has to pick up X,Y,Z off set for new set up, tools are already in the rack.

when we first get the presetter i was old school and sounded just like you.
but after using it for awhile i'm now a believe and don't want to the old method anymore.

when the toolsetter broke down we used a hiegth gage and an indicator to achieve the tlos instead of the old method.

if your using the tool setting probe, then i agree, the cycle takes longer than just setting them by hand, but an offline toolsetter is the way to go.

[Neal]

Personally, I'm not a fan of the tool presetters. I understand the concept as to why they are used. My only issue is that IF the fixture offsets are not programmed correctly AND the cancellation of the Tool Length offset are not carefully considered, you might be in for a big crash.

Neal