Tool offsets clarification

[vw_chuck]

Reading through the lathe manual and I have some questions on too offsets. It says you will have a reference that will have a 0 in the x and z offset indicating that it is the reference tool. The confusion is that the manual talks about setting a reference tool for OD tools and then a reference tool for ID tools. How does the software know which reference tool to use? Does it just look for the OD or ID tool with 0,0 for x and y offset? Or is there a x Diameter reference and Z reference for each tool but it is not displayed?
Having a hard time getting my head around tool offsets between OD and ID tools

[Dave_C]

How does the software know which reference tool to use?

Short answer, it doesn't!

Setting tools for the lathe is not as simple as setting tools for a mill because upon startup, your tool may or may not be cutting the proper diameter on the part.

Generally speaking, we use tool number 1 as our OD reference tool. That mean that this tool will have no offsets for X and Y because there is nothing to offset from, it can't be offset from itself! (so therefore we will now offset all other tools from this one)

Assuming no two tools will have the same X and Y dimensions, they will therefore cut at different diameters and different Z positions. We still however, need to establish where our reference tool, also known as "master tool" is cutting after we started up our machine. So we take a skim cut on a piece of scrap, measure that cut without moving the tool in X and then enter that measurement as our reference.

From there just follow the steps in the manual for each additional tool and touch off as needed or use a touch off tool that will enter the numbers automatically.

So to answer the rest of your question, an ID tool can not use the OD tool as a master because you can't touch off on ID tool on the OD of the part. So you will have to establish a reference for the ID as well.

Start with OD tools first, get that procedure in your head and then we'll mess it all up again when we try to explain how to do ID tools, LOL

Dave C.

[vw_chuck]

The confusing part is that there will be an OD tool with 0,0 for offsets and an ID tool for 0,0 for offsets. How does the software know which one to use as the reference? Also if your z axis reference is different between the OD and ID reference how does the software know this? Ah more confusion. I think the directions are far too dumbed down. I need to know exactly how the software is figuring things out.

[Dave_C]

I need to know exactly how the software is figuring things out.

You have to tell it what you are doing. You do this when you set up a tool to "approach from the front" and give it a tool pointing direction.

The software is pretty smart as long as you choose the proper "approach from" direction and tool pointing direction.

We just did a long discussion on how to set up boring bars a week or so ago. Here is the link. : viewtopic.php?f=60&t=4833

Dave C.

[cncsnw]

Where does the manual say that you "set a reference tool" for ID tools?

What it should say is that you have one reference tool, and you use the reference tool to set a reference diameter (X reference, or "X Diam" on the screen) in preparation for measuring OD tools; then you might need to use that same reference tool to set a different reference diameter in preparation for measuring ID tools.

There is only one reference tool. In some procedures the reference tool is imaginary and arbitrary, but assuming your procedure is to use a physical reference tool, it needs to be the same one for all measurements: OD and ID.

To reiterate: if you use a physical reference tool, you might use it to set X reference ("X Diam") at different places in preparation for measuring different types of tools, but you always use the same reference tool.

[vw_chuck]

Dave C yes I was on that thread and the second video that was posted clearly shows the problem. The guy that made it selected ID tool and it gave him the WRONG offset. So you guys keep saying the software knows but in this video it clearly does not know.
https://youtu.be/sGTc99IgwcU

[vw_chuck]

I wish there was an actual Centroid video showing how to do EACH type of tool from start to finish.

[Dave_C]

Dave C yes I was on that thread and the second video that was posted clearly shows the problem. The guy that made it selected ID tool and it gave him the WRONG offset. So you guys keep saying the software knows but in this video it clearly does not know.

I watched this video a couple of times, not sure what he is doing wrong because I use that EXACT same method with my touch off tool and it sets all my OD and ID tools just fine.

He may have an issue with his X reference diameter not being set right because he says "It does not matter if the tool setter is on centerline" (or some comment along that line)

It does matter if you are going to set both ID and OD tools from the same setup. For example my touch off probe is .250" in diameter. I touched off all of my OD tools from the front side of the tool and then touched off my boring bar tools and my ID threading tools, from the back side of the probe.

I made some adaptors afterwards and all cuts and threads came out right!

There is nothing wrong with CNC 12.5, it works, you just have to make sure you set your references correctly.

Use the master tool to set the X and Z part references first so the reference tool has (0's) in both the X and Z in tool offsets.

In the video above, he has all the right settings for ID tools. (tool 4) These have to be set to "ID", "Approach from the front" (you can't change that one unless you have gang tooling set) and "2" for direction. And if your references are set properly you will get good tool offsets.

I understand this subject is a bit hard to get your head around and the manual doesn't help much because it is written for a rear tool post.

Again, set your X and Z part zero using the reference tool, then set the reference to whatever diameter you are touching off on. Then use the front for OD tools and the back for ID tools.

Dave C.

Edit: If you look in the lower left corner of the tool offset page, you will see what your reference diameter is set to!

[vw_chuck]

Dave I went back and verified my setup as i also got a huge negative number for my x offset on my boring bar. I MDIed over to 0 with my boring bar and it landed right on centerline so yes it did seem to work for me. Not sure what the guy in the video did wrong
I guess if you touch off and it is a negative number the software realizes you are on the other side of the touch probe.

[Dave_C]

I guess if you touch off and it is a negative number the software realizes you are on the other side of the touch probe.

BINGO!

I told you it was confusing, but you figured it out! You do get a negative number because you are across the centerline of the coordinate system. X+ is on the operator side and X- is on the backside.

Glad you got it working.

Dave C.