[partsman]

Ok... I lied. It IS another stupid offset question

Go easy on me.. I'm still learning but I just can not get my head around the way HAAS handles the Z offset.

I'm only familiar with the Mach software where you loaded your tool into the holder, touched the tool to your work, & clicked Z zero (or something like that). I've been reading for three days and all of the instructions that I have seen for the HAAS require you to add or subtract the position in one line from the offset number in another line... or something like that. Everyone says never use the 'part zero set' for the Z or you will crash. Why is that? What am I missing?

I figure it is cheaper to ask here than break a few tools trying to learn what everyone else seems to already know.

Thanks in advance!

[Geof]

You have been reading the wrong stuff.

Here is the sequence I use (Most times):

Push HAND JOG

Push OFFSET

Now you should see either TOOL OFFSET screen or the WORK ZERO OFFSET screen. You can toggle between the two by pushing OFFSET.

Make sure there is no entry in the Z column of the WORK ZERO OFFSET screen.

Toggle back to the TOOL OFFSET screen.

Bring your first tool down to the part using the paper feeler gauge method.

Check that the cursor is on the line for the tool you are touching off.

Push TOOL OFSET MESUR. If you look at the bottom of the screen you will see Z POSITION, the value here will transfer to the line the cursor is on.

Push NEXT TOOL. The machine will change to the next tool and at the same time set the Jog Handle speed back to .01.

(If you push any key between TOOL OFSET MESUR and NEXT TOOL the tool change does not happen.)


There are variations on this method if you are using a toolsetter or a reference surface but this will get you going. Ignore anyone who rants on about a more complicated method until you has this procedure down pat.

[Machineit]

Ya, just do what Geof said and jog your tool down to the part or your setting fixture. When you get it set at the height you want. Then go to the OFFSET page. Highlight the tool that you are setting and push tool offset measure. If you are using another tool then push next tool and set it the same way.

After you have touched off all of your tools, then add you fixture height if needed. What I mean is that if you used a 4" touch-off gauge to set them, now is the time to add the gauge height to each tool, such as -4.0" and enter.

Keep it simple until you are confident.

Mike

[txcncman]

Ya, just do what Geof said and jog your tool down to the part or your setting fixture. When you get it set at the height you want. Then go to the OFFSET page. Highlight the tool that you are setting and push tool offset measure. If you are using another tool then push next tool and set it the same way.

After you have touched off all of your tools, then add you fixture height if needed. What I mean is that if you used a 4" touch-off gauge to set them, now is the time to add the gauge height to each tool, such as -4.0" and enter.

Keep it simple until you are confident.

Mike

Why are you adding gage height? Are you attempting to make the tool read zero when it touches the table? If so, why?

[Geof]

As I said above ignore both of them until I say you can read them.:stickpoke

[partsman]

As I said above ignore both of them until I say you can read them.

LOL!!! I think this is how most of the other posts that I was reading ended up

Thanks Geof!!

Ok... so I set all of my tool offsets from an empty spot on the table somewhere using your method. Now I want to load a part in the vise. How do I get the top of the part to Z0? I want to load up tool #1, bring it down to the top of my part and............


.

[Machineit]

Why are you adding gage height? Are you attempting to make the tool read zero when it touches the table? If so, why?

The gauge is on top of my PART!

[txcncman]

The gauge is on top of my PART!

Ah. Ok. I get it. No need to change every single tool length offset though. Unless you just like pushing a lot of buttons and risking mistyping a number once in a while. Just use the work offsets to shift all.

[WallyL7]

This AGAIN???

[KenFoulks]

Ok... so I set all of my tool offsets from an empty spot on the table somewhere using your method. Now I want to load a part in the vise. How do I get the top of the part to Z0? I want to load up tool #1, bring it down to the top of my part and...

This is exactly what machineit was referring to, touching your tools off a common point. It is usually unlikely to be the table because shorter tools may not be able to reach the table. Let's use the vice jaw as an example:

Step 1: Ensure setting 64 is OFF
Step 2: Follow Geof's steps (Using TOOL OFFSET MEAS for each tool while touching the top of the vice jaws.)
Step 3: Take any of the tools and touch the top of the part.
Step 4: Toggle the offset screen to the work offsets.
Step 5: Press PART ZERO SET for the offset (G54) you would like to use.
Step 6: Subtract the tool length (-16.000-(-18.000)=2.000)
(For step 6, -18.000 is the distance from machine home to the top of the vice. -16.000 is the distance from machine home to the top of the part. 2.000 is the difference.)

[partsman]

Thanks Ken,
But... now we are back at doing math. It sure seems like the HAAS should have a way to do that math for you. Is there not just a button you can press to fill in that field... and if not... why not?

Sure... 16"-18" does not leave much room for error but real world numbers like 16.036" - 18.558" leaves a lot more room for error 1)- typing those numbers into a calculator and then 2)- typing the result back into the control.

[haastec]

I'm only familiar with the Mach software where you loaded your tool into the holder, touched the tool to your work, & clicked Z zero (or something like that).

You can do this exact same procedure with the Haas, it's just not the most efficient way if you are using the a lot of the same tools for multiple jobs.
This is what Geof described in his first post. However, you modified what he told you and touched off an empty spot on the table. Now you just introduced a different method. (Read Geof's second post)

BTW, there is math involved with machining, that's just the way it is.

[KenFoulks]

1)- typing those numbers into a calculator and then 2)- typing the result back into the control.

You can put your calculator away. After PART ZERO SET, subtract the tool length by typing in the tool length and pressing WRITE/ENTER. Done. (WRITE/ENTER adds the input value to the current value)

Haas has made it very simple, we call it probing. If you want a less expensive option, touch the tools off the part and use a single button (PART ZERO SET). If you want to touch the tools off of something other than the part, be prepared to tell the machine what you just did.

[txcncman]

"...be prepared to tell the machine what you just did."

I love it!

[partsman]

You can put your calculator away. After PART ZERO SET, subtract the tool length by typing in the tool length and pressing WRITE/ENTER. Done. (WRITE/ENTER adds the input value to the current value)

Haas has made it very simple, we call it probing. If you want a less expensive option, touch the tools off the part and use a single button (PART ZERO SET). If you want to touch the tools off of something other than the part, be prepared to tell the machine what you just did.

Perfect! That is exactly what I was looking for.

Thanks again!

[Pondo]

My trainees had a very hard time learning the different machines until they understood what the numbers actually are and how the machine is using them.
We have many different machines that are set up differently - VBMs turning centers, 3- 4- and 5-axis machining centers, and CNC machines from a 1 year old DMU 5-axis mill to a 40 year old G&L punch tape reading lathe. There are at least 5 different offset systems on the CNC turning machines alone.
Once they understand what the numbers mean, it becomes very much easier to learn the different machines.
The more trainees rely on the monkey see - monkey do way of memorizing "I press this button, then this one, and then type in this number" the worse they do.
The way I explain it, I home the machine. Then I explain that if no offsets were applied, it would try to run the shape of the part as if the tip of the tool were at X0, Y0, Z0. The offsets are exactly that - how far it is from that home position to where the tool tip would be at the part's X0,Y0,Z0. There are many ways to come up with that info. You can set offsets from tools only, G54 offsets only, or both. Tool lengths can be positive or negative and so can G54 offsets. The total of G54 and tool offset just has to add up to equal the distance from the tool tip at the machine's home position and the tool tip at the part 0 (or WPC as we call it).

[Machineit]

My trainees had a very hard time learning the different machines until they understood what the numbers actually are and how the machine is using them.
We have many different machines that are set up differently - VBMs turning centers, 3- 4- and 5-axis machining centers, and CNC machines from a 1 year old DMU 5-axis mill to 40 year old G&L punch tape reading lathes. There are at least 5 different offset systems on the CNC turning machines alone.
Once they understand what the numbers mean, it becomes very much easier to learn the different machines.
The more trainees rely on the monkey see - monkey do way of memorizing "I press this button, then this one, and then type in this number" the worse they do.
The way I explain it, I home the machine. Then I explain that if no offsets were applied, it would try to run the shape of the part as if the tip of the tool were at X0, Y0, Z0. The offsets are exactly that - how far it is from that home position to where the tool tip would be at the part's X0,Y0,Z0. There are many ways to come up with that info. You can set offsets from tools only, G54 offsets only, or both. Tool lengths can be positive or negative and so can G54 offsets. The total of G54 and tool offset just has to add up to equal the distance from the tool tip at the machine's home position and the tool tip at the part 0 (or WPC as we call it).

You are absolutely correct. The most important thing in teaching someone anything is explaining WHY it is done! Whether I'm teaching someone something on a computer, to run a machine, or anything else I explain WHY it is done that way.

Those who just want to learn what buttons to push soon end up in trouble.

Thanks Pondo!

[haastec]

My trainees had a very hard time learning the different machines until they understood what the numbers actually are and how the machine is using them.
We have many different machines that are set up differently - VBMs turning centers, 3- 4- and 5-axis machining centers, and CNC machines from a 1 year old DMU 5-axis mill to 40 year old G&L punch tape reading lathes. There are at least 5 different offset systems on the CNC turning machines alone.
Once they understand what the numbers mean, it becomes very much easier to learn the different machines.
The more trainees rely on the monkey see - monkey do way of memorizing "I press this button, then this one, and then type in this number" the worse they do.
The way I explain it, I home the machine. Then I explain that if no offsets were applied, it would try to run the shape of the part as if the tip of the tool were at X0, Y0, Z0. The offsets are exactly that - how far it is from that home position to where the tool tip would be at the part's X0,Y0,Z0. There are many ways to come up with that info. You can set offsets from tools only, G54 offsets only, or both. Tool lengths can be positive or negative and so can G54 offsets. The total of G54 and tool offset just has to add up to equal the distance from the tool tip at the machine's home position and the tool tip at the part 0 (or WPC as we call it).

Very well put to a very common problem.

[partsman]

First... I just want to thank everyone again for contributing! :cheers:

Pondo = awesome explanation!

The offsets are exactly that - how far it is from that home position to where the tool tip would be at the part's X0,Y0,Z0. There are many ways to come up with that info. You can set offsets from tools only, G54 offsets only, or both.

So then if I set all of my tools from the top of my vise and my work is 0.5" above the top of the vise- do I not just add 0.5" to the G54 Z offset?

Is there anyway to check my work without actually crashing a tool. I though the current position screen's G54 display should show Z0 at the top of the part but every tool but the tool used to set the offset is waaaaay off. Maybe that is not the correct screen to look at???

[Geof]

....Is there anyway to check my work without actually crashing a tool....

I use Graphics with Single Block on and the Machine Coordinate display. You get to the Machine Coordinate display in the Graphics screen by pushing F3 to toggle through the four displays; Machine, User, Distance to go and Work.

Step through the program until the tool reaches Z0. and read the Machine Coordinate Z value, then Handle Jog to this position and check that it is at Z zero on the part.