Z travel exceeded and other mysteries

[cnckeith]

you can use any tool as the reference tool. I use tool 1.

tool 1 is not longer or shorter than itself.. so the offset values are zero for tool 1

[ScotY]

Can you post a picture of your tool offset page?

[cnckeith]

im not near the lathe at the moment.. i've asked one of the centroid techs to post it.

[ScotY]

Thanks...well, I have zeroed out the offset values for tool 1 and then tried to measure tool 2 and something is not right. Back to reading the manual...

[cnckeith]

dont forget to set the reference while tool 1 is at the skim cut or touch off position. this tells the control to "remember" that position for measuring the other tools.

[cnc_smith]

[ScotY]

Hmmm...I'm still doing something wrong. I finally understand the Z offsets...that is sorted. However, what happens when you want to add a new tool at a later date? I'm assuming you must first touch off on Z for the reference tool (possibly at a new reference position), then use this Z ref position to set up the new tool? Won't this throw off the values for the other tools?

My X offsets look like they are all still referenced to a distance from machine home. In other words, the reference tool 1 offset is about -4.0, a longer tool #3 is about -3.0, etc. Here's what I did...

Using tool 1 (my reference tool), I touched off the tool on my stock, measured the stock, and used that as the X diameter. Then I measured the X offset there and saved. This input the -4.0 value as mentioned above. The -4.0 is 2 times the physical distance from the tool tip to the machine home position so it makes sense, but it does not show zero for the reference tool as shown in the pic posted by CNCSmith (I'm assuming he's a Centroid guy and those settings are from your shop lathe, or if he's not, then those settings are what comes in the CNC12 app before you delete it like I did). It says in the manual on page 4-9 that when you measure the first tool in X (it does not mention reference tool here) it will insert a value into the X offset column and figure 4 shows a value of 1.0. So, now I'm completely confused.

Anyway, the way I have it set up now SEEMS to work but I figure if I'm going to learn how to do this, I may as well learn it the proper way.

[cnc_smith]

"However, what happens when you want to add a new tool at a later date? "
If you are adding a new tool later you can bring the reference tool down, reset the reference Z with the reference tool if you do not have the same reference surface for Z to touch off of. Then bring down the new tool to the new reference surface or the same reference surface if it has not changed then measure the new tool. This will not through off the values for the the other tools. All you have done is told the control this is the new surface that the new tools will be touched off of.

"My X offsets look like they are all still referenced to a distance from machine home."
Not sure how you set Part X0.0. I am going back to basics how I first set Part X0.0 and setting X Reference for the first time. Part X Zero is set to the center line of the spindle. You may have done these steps already that I am going explain. The reference tool the X and Z tool offsets should be set to Zero. Make a skim cut with the reference tool. DO NOT move X, just move Z back so you can measure the diameter From the main screen press F1 -Setup, F1 - Part, F8 Set X. In "Part position" enter the diameter you measured. Arrow key over to "Tool Number" and enter the number for your reference tool. Arrow key over to set "All WCS" and press the space bar to toggle to Yes to Set All WCS then press F10 - Set. Next Press the ESC key two times. This will bring you back to the Setup screen. Press F2- Tool Offset. Arrow key over to X Offset column. Press F1 X Diam key. Them Press F10- to save Reference Position. The diameter you had measure is what the value should be displayed. Now Press F2 Measure tool, F5 Measure offset X, F10 Measure here. The offset for X should still be Zero if everything was done correctly. Then you can measure all the rest of your tools. The X offset for each of the other tools should be the difference in length from the reference tool. They can be positive or negative values.

One other note when you are setting the X Diam or Z Ref you will notice that there is a second option to type in the value for the X Diam or Z Ref. For X Diam. if you know the diameter that you will be touching the tools off of you can type the known diameter in instead of having to bring the reference tool down to touch of the X Diameter. For Z Reference Part Z Zero needs to be set first then you can type the Z value of the surface you are going to touch the tools off of.

[ScotY]

Ah, okay...I have not set X zero in the part zero menu. I think now I understand what I’m supposed to be doing. I will try again this afternoon and see if I can get it working.

Thanks for taking the time to write that all down. That is why I needed Keith to make a video.