Tool height offset not transferring to job - resolved

[kb58]

I'm just starting out making elementary moves with my router. I decided a first try would be to use Intercon to program drawing a square on a piece of paper with a pencil in the spindle. I followed the excellent tutorial video Centroid made 10 years ago (https://youtu.be/mA41pUyONJM?si=bYEUIqWn0llFhjHV) and entered the "tool" into the library. Yes, I realize what I'm doing doesn't require this but it's to expose me to the work flow. Anyway, the tool offset in Setup > Tool > Offset Lib was set to -86.307 mm. It was Saved off, and reads correctly if the page is revisited, however over on the CAM tab, when I click on Modify the Tool #1 entry, the displayed tool height is both grayed out and has a zero value. Running the simple job confirms that it's ignoring the tool offset in the Tool menu. I know it's something I'm doing wrong but can't see what it is. Thanks.

[kb58]

In the Centroid video, when he goes to the job listing and the tool entry, it does show the expected offset, but it's grayed out. I understand why, but not why mine is stuck at zero.

[kb58]

Hmm, not marking this as resolved, but I found that if I enter the exact same values for Tool "2", it is properly referenced from the job. Is there something different about tool #1? Nothing was mentioned in the video and as was said, it worked fine for them.

[tblough]

You have tool height offset set to 0. Change that to 1 to use H001 as the offset.

Tool height offsets and diameters are independent of the tool number. You can load tool 1 and height offset 32 and diameter 14. That is why there are separate entries for height offset and diameter offset

[kb58]

See next post.

[kb58]

I understand that tool length is set in Setup > Tool > Offset Lib and is the physical length of the tool to a known reference surface, no problem there. I guess I don't understand what "tool height offset" is. The word "offset" confuses me. What is it in reference to, as it's an integer, so must be referring back to the Offset table in some way.

On a related note, tool length is as defined above, fine, but where does the offset live that tells it how much further Z must travel before reaching the surface of the work? Must it be entered in every line of the job when setting cutter depth? Seems unlikely, that it must live as a global offset from which all other cutter actions reference.

Apologies for the beginner question, and yes I did read the manual but I'm still not getting it.

[cncsnw]

The height offset number (H) and diameter offset number (D) are indexes into the offset library. They tell the control what lines of the offset library to look on, to find the current length and diameter of the tool, respectively.

The value of the height offset is grayed out in the Intercon Tool Change screen, because it is generally not useful to type in a number for the tool height offset. Instead, before you run the job, you go to the Offset Library and measure the length of each tool that you will be using.

The CNC job does not contain the value of the length offset anywhere. The CNC job just says something like "G43 H2", and when the control runs that job, and gets to that line, it looks up the current value of H2 from the Offset Library. Therefore you do not have to change the CNC job just because the length of the tool has changed. Just measure a new height offset in the Offset Library, and run the job again.

This might help you visualize the flow:
http://www.cncsnw.com/UserMenus.pdf

Note that it is not necessary to set up and measure your tools before you write the part program; but in my experience, that is a good way to find out whether you actually have the desired assortment of tools and tool holders.

[kb58]

I think it's becoming clearer, that "Tool #1" should not be considered the physical tool, but an index to pre-assigned offsets and diameters, is that correct? I was over thinking this, like usual.

The (rather critical) part I was blanking out on was setting the stock location. That was the missing piece for me, that while the above sets the spindle-to-tool-tip distance, I didn't see where the rest was accounted for, the tool-tip-to-work offset. Thank you very much.

[tblough]

I think it's becoming clearer, that "Tool #1" should not be considered the physical tool, but an index to pre-assigned offsets and diameters, is that correct? I was over thinking this, like usual.

It's the opposite. Tool #1 is the physical tool. Hnn and Dnn refer to virtual "bin" numbers that hold offset distances and diameters. You can choose to associate H01 and D01 with tool #1 like many people do, but you don't have to. You could just as easily use tool 1 with H09 and D12.

It's common to use one diameter offset for roughing and another for finishing with the same tool. If I'm thread milling, I can have one diameter offset set to 0.030" oversize, one set to 0.010" oversize, and the finish pass uses an offset that I've determined through test cuts to give me the correct finish size. I use the exact same g-code for all three passes and just call G41 D01 before the first pass; G41 D02 before the second pass; and G41 D03 for the finish pass.

[kb58]

So the H and Ds are simply often-used heights and diameters that are assigned to whatever physical tool matches. Got it. I'm just trying to build on a solid foundation instead of a house of cards. I know that you guys are constantly pinged about elementary things you learned years ago, but we all start somewhere! Thanks again.