What's new
What's new

proper way to set z height for face milling rough cut parts

Not really, see you just said, you needed to go in and set that parameter, I don't have to. but you have to every time.

It does not work like you assume. Each time you create a new toolpath you need define its parameters no matter which software you use... right?

Mastercam has a tab called "linking parameters" within nearly all toolpaths. This is where you set the depth of the feature, top of stock for that feature, tool retract height and clearance height.

You can leave these as defaults if you want, or you can go back into the tool path parameters and change them however you'd like, it only takes 3 or 4 mouse clicks.
 
Or just go maybe .450 deep on the first pass on tall parts. What could go wrong? :D
I had this happen to me while running a demo at a trade show in front of around 15 people. We ordered pre-cut material and one of them was about .3" longer than it should have been which isn't noticable when it's a 40lb piece of 4140. The 6" shell mill almost made it through the cut until it ripped it out of the jaws.
 
I don't think I've ever seen a print where the depth of a hole is referenced from the opposite face.
I have. Can't say it was Best Practices or anything but I can think of at least one job where it made sense - was a sort of manifold thingy where the cross holes had to be at a fixed dimension from one edge so the depths of the intersecting holes was controlled by a dimension from the opposite side. Was that confusing enough ? If not I can try harder, but you probably get the idea :)
 
I have. Can't say it was Best Practices or anything but I can think of at least one job where it made sense - was a sort of manifold thingy where the cross holes had to be at a fixed dimension from one edge so the depths of the intersecting holes was controlled by a dimension from the opposite side. Was that confusing enough ? If not I can try harder, but you probably get the idea :)
Yup, me too, a manifold also, six sided full of a million different holes, some datum's relative to basackwards surfaces, good times! :DUntitled.jpg
 
Last edited:

Ok, one last real world example...

Capture111.JPG

I am currently running a set of soft jaws to hold this and programming the milling op for the parts as we speak.

Final OP; face off the extra stock on top and then cut the notch to create that tang on the left side of each piece.

The overall part height is +/- 0.01 and the tang thickness is +/- 0.003.

1.) Where would you pick up your z reference?

2.) Where would you set G54 Z0.0?
 
Ok, one last real world example...

View attachment 416826

I am currently running a set of soft jaws to hold this and programming the milling op for the parts as we speak.

Final OP; face off the extra stock on top and then cut the notch to create that tang on the left side of each piece.

The overall part height is +/- 0.01 and the tang thickness is +/- 0.003.

1.) Where would you pick up your z reference?

2.) Where would you set G54 Z0.0?
Standard daily operations, I use the Haimer touch it off on the bottom of the soft jaw step, then type in +(height of finished part) in the G54 Z
What I think newb's don't understand because they don't shift work coordinates ever is, you are still relative to the bottom solid immobile datum, your cutting tools will go to EXACTLY the same position either way,
the difference is in the programming, and the relative numbers you see in your Gcode.
I think idiots are thinking we are setting the Z RELATIVE TO THE TOP OF THE STOCK, NO relative to the bottom immobile datum still.
 
Ok, one last real world example...

View attachment 416826

I am currently running a set of soft jaws to hold this and programming the milling op for the parts as we speak.

Final OP; face off the extra stock on top and then cut the notch to create that tang on the left side of each piece.

The overall part height is +/- 0.01 and the tang thickness is +/- 0.003.

1.) Where would you pick up your z reference?

2.) Where would you set G54 Z0.0?
Another classic I use, because injection mold plates and inserts have to be such a tight tolerance in height,
with the hat/stock on the top as you have here in this example,
I will put in a face mill, manual across the top removing a couple thou, then while the part is still in the machine I mic its overall height.
I take the mice'd dimension minus part needed dimension will give me exactly within .0001 or so from my desired height when I run the face mill.
If that makes you even more con-fus-ed.
 
I think idiots are thinking we are setting the Z RELATIVE TO THE TOP OF THE STOCK, NO relative to the bottom immobile datum still.
I asked you that pages ago. It's again--an idiosyncrasy of Gibbs or maybe something you like to do. It's just as easy to call that surface zero and then any operation that goes below zero had better have clearance under the part. Easy-peasy. You took it as an affront to your intelligence or something.
 
Ok, one last real world example...

View attachment 416826

I am currently running a set of soft jaws to hold this and programming the milling op for the parts as we speak.

Final OP; face off the extra stock on top and then cut the notch to create that tang on the left side of each piece.

The overall part height is +/- 0.01 and the tang thickness is +/- 0.003.

1.) Where would you pick up your z reference?

2.) Where would you set G54 Z0.0?
Probe the top of the fixed soft jaw blank for G54 Z0 (be sure to hammer the jaw down first, so it can't move if you tap your parts in later). Program everything to run from there. I usually have to raise Z0 a thou after cutting the soft jaws to get the part height dead nuts.
 
Also here is the other reason, if you set the Z Zero at the top of the finished part, then regardless of how tall the part is your standard unchanged clearance moved will always clear, and lessen machine crashes.
Why?
Most software has a default parameter for everything, its either zero, or a default from a setting parameter, or a template default....
Most software has at least 2 clearance planes, one global and one local.
If you program from the bottom, you have to change all these clearances every time, some how, different ways different software.
My CAM program (GibbsCAM) has a global clearance, I set to .1 , and then in each operation I create its local clearance value is defaulted to the value that was last used, So I set this to .1 also, and It will stay there endlessly until I change it.
So I never have to change clearance, EXCEPT If on my first OP there is a big ass chunk of material to remove like OP mentioned, then I will set as reference to his situation of .5 extra material, I set global and local clearance to .6
This is the main thing I have changed in many shops that has drastically lessened machine crashes.

If you program from Bottom and all your heights are a hard number from Origin, then you will need to change them, no argument there. However that is a trash workflow regardless. Doesn't matter if your origin is top or bottom, hard numbers from any fixed position will require changing values.

A more robust workflow, if your CAM allows for it, is to set your Clearance plane to Stock Top plus a desired value, Retract plane to Model Top (or Stock Top, depending on how early on you rough the top of your stock) plus a desired value, Feed height to Model Top plus a desired value (if you want to use Z feeds, or just disable it if you're plunging in air), Top Height to Model Top and Bottom Height to the top of your workholding plus a desired clearance value (if you're using workholding in your CAM environment). If you're not using workholding in your model, then select Stock Bottom plus a known value to clear jaws/clamps/dovetails/etc. This is why it is advised to throw your part file into a template file that has all of your workholding/etc built into it with these planes tied to the models. 90%+ of the work is done already at that point and all the details can be output on your setup sheets for whoever is in the shop.

Once you define those height planes, set these as user defaults, and you'll never need to change them ever again, regardless of your stock size, part size, etc as these values are now tied to parameters that change with your part setup in CAM.

Not all CAM software allows this but many do and if you get creative with your workflow you can build systems that require little to no user input aside from dropping a model into a file, adjusting your stock size in CAM to match worst case at the machine and regenerating it. Simple regen doesn't cover all part geometries but it will get you very close in most cases and mitigate most of the wasted, repetitive motion when programming parts, as well as make your process more stable and more reliable.
 
I asked you that pages ago. It's again--an idiosyncrasy of Gibbs or maybe something you like to do. It's just as easy to call that surface zero and then any operation that goes below zero had better have clearance under the part. Easy-peasy. You took it as an affront to your intelligence or something.
BUT, If you raise it up to the TOP OF THE "FINISHED PART HEIGHT", all your GCODE WILL SHOW EXACTLY THE CORRECT Z DEPTHS FOR HOW DEEP ALL TOOLS ARE GOING INTO THE PART, Nothing to do with Gibbs or software, separate subject.
I swear this is not that difficult to understand!
 








 
Back
Top