CNC Tool Length Offsets Explained

This video is talking about the 3 most common Tool Length Offsetting methods used on CNC milling machines, and the pros and cons of each method.
Method 1 - For this first method, you will assemble the tool and load it into the spindle of the machine. Your part would also be loaded into the vise/fixture. Next, you'll bring the tool tip down to the top of the part (or where ever you plan on placing Z0). To accurately set the tool tip to the work, a piece of paper can be used. Once the position is established, make note of the distance from HOME the machine is currently at. This will be the value that gets loaded into the height offset for this tool. A value of 0 will be input into the Z value for the work offset (G54).
This method is quick as only one touch off is needed for the tool, none for the work. The limitation of this method is it is only good for the current part. A new part (one that differs in thickness) will require a new tool touch off. Tool length is a large negative number, work offset is 0.
Method 2 - This method is similar to Method 1, with the addition of an intermediate block. This block can be of any thickness and can be placed at any position in the machine, as long as the same block and position are used for all tool and work settings. Touch the tool tip to the top of the intermediate block. The distance from HOME to the current position will be placed in the tools height offset. Next, measure the height difference between the intermediate block and the work piece. There are several methods to accomplish this, but again paper can be used. The difference is height between the intermediate block and the top of the work piece will be entered into the Z value of the work offset. Polarity of this number is very important.
This method requires a touch off for each tool and one touch off for the work piece. If a new work piece is loaded, simply re-measure from the intermediate block to the work piece, no need to retouch the tools. Tool length is a large negative number, work offset is difference between intermediate block and work.
Method 3 - This method is my preferred option as it results in an offset that is the physical length of the tool (a positive number). With no tool in the spindle, bring the spindle face to the work piece. Paper, again, can be used. With the spindle at the Z0 location on the part, this distance from HOME will be loaded in the Z value of the work offset. While at this position, you can zero out the Relative position field for Z. Then move the spindle up, load the tool, retouch the same position. The value in Z is the actual length of this tool. That value will go into the tools height offset. Repeat for all tools.
This method requires a touch off for each tool and one for the work piece. If a new work piece is loaded, simply re-measure spindle face to top of part. The tool length is a positive value that is the tools physical length.
Positive tool lengths can be transferred from machine to machine. Negative values cannot. You can quickly check a positive tool length with a tape measure/caliper. Negative values cannot.
If you do not like using paper for touch offs, and you do not have a probe, I would recommend something similar to the setter below. You can set the '0' to be at exactly 2.00, and there is some compression to the plunger on top which helps to cut down on touch off mistakes.
See other blog posts
blog.caminstructor.com
Check out our website
caminstructor.com
#Mastercam #LearnCNC

[@jczon7]

After 12 years working with cnc mills, I can say now I know the difference! I have used those methods but never understood exactly what the did it that way

[@actiontower]

am new to all of this. But for 2 long months NO one and NO One on the internet Explain this as understandable as You ! thank you from the bottom of my heart ^_^ too bad i can't like this video more than once ^_^ .

[@CamInstructor]

You are so welcome!

[@jeremyalgier7843]

Thank you for making this video!!! This really helped me understand tool length offsets and got me running my first machine without a hitch.

[@CamInstructor]

Glad it helped!

[@amirb3083]

I wish I could click on like button thousand times. Thanks so much.

[@CamInstructor]

Wow, thank you!

[@practicemakesbetter7132]

Excellent video, thanks for sharing!

[@CamInstructor]

Glad you enjoyed it!

[@bigbattenberg]

Great explanation! I jus started as a CAM programmer (Hypermill) for turning and milling but I have no CNC experience in practice and no CAM experience. So I'm digging through the manuals of the Okuma lathes for starters (there is the most need in the turning department) and understanding offsets is a vital aspect. In fact the big Okuma has a VDI QC tool holder system and yet they have used the 'master tool' system which is not very smart. Working from a fixed tool holder interface is the way to go. You point out that probes have a known length, the same must go for lathe probe arm systems. I have been looking at some Haas videos on their probe arm system. I have yet to understand fully how it is calibrated and which offset numbers are put into the offset table.

[@WhyDidYTstartThisHandleShit]

holy crap this is awesome. instead of me explaining this to people, maybe i should just show them this vid instead.

[@CamInstructor]

For sure!

[@education-finance]

I like 👍 this job

[@cheizaguirre5494]

If i use method 3 that new value on the operator is the number i will use in the offset geometry for length ? Thanks for the video

[@sydneymwale1070]

Wow this is a video I need help on the tool offsets please, kindly share full videos on tools offsetting, step by step please?

[@mitchanderson9858]

In the first method, I like to think that the tool length offset isn't meaningless, it's just that "tool length" is a bad description. I think "tool distance offset" is a better description since its the distance from the bottom of the tool to the top of the part. In the second method, we have a "tool distance offset" and setting G54 is like a "distance correction offset."

[@user-xb1ht4py2v]

I spent days trying to find a good explanation of this and yours is by far the clearest and best explained. Which method works best for multiple tools and mutiple setups for the same part? And How would it work if you used method #2, but the arbitrary "block" had a height equal to the height of the spindle (16" in your ex.) ?

[@CamInstructor]

2 or 3 would work for multiple parts, each part would have its own work offset (g54 g55...)

[@raymondzhao9557]

cooooooooooool

[@173roberto]

If I take a height Gage and measure the distance from the part to the machine's table, what method should I use?

[@CamInstructor]

This would be the second scenario. Sounds like you're just removing the block shown in the video. I guess you are touching your tools directly to the table? Or do you touch them to a block, measure your work piece and then subtract the block height from your measured height?

[@actiontower]

what if we use scenario No.2 but instead of using 246 Block we use imaginary block that length is equal to the distance between table surface and the tip of the Bit.(it would be 14 inch in your Example) i think that mean T length would Be T=0; (the other tools would be T2=T2-T1, T3=T3-T1 , T4=T4-T1 .....) and G54 Z= Z value when you touch the tip to the surface of the work piece.(it would be -10 inch in your Example) would this work ?

[@CamInstructor]

Yes that would work, the math checks out.

[@JustMe-er9ve]

Why not touch the tool off to the table(Hx) and use an dial indicator from the table to the top of the workpiece(G54)?

[@CamInstructor]

You would still need to use something to gauge when the tool is 'touching' the table. Using a piece of paper for this would be the same as using the 6" block in the video, just the paper is ~0.003" think instead of 6". So steps would be the same as scenario #2.

[@JustMe-er9ve]

@@CamInstructor Yes, I use a 1,2,3 block.

[@henmich]

How do you measure the spindle face to the work?? That would terrify me. Here, let me just bring my expensive spindle down and hit it on the stock. So then what? Use a shim? I'm curious to know how this is done.

[@CamInstructor]

Would be no different than touching a tool tip off to a workpiece. Yes, most will use some sort of shim be that something small like a piece of paper or something larger like a gage block or 1-2-3 block.

[@gertkristensen6451]

best way set you tools from tabel . you can use g54 ,, 55 ...56 just set you offset in tabel .. G54 55 56 from tabel to top off you parts ..all tools works

[@CamInstructor]

The table works, the tricky part is knowing when the tool is touching the table. This is why we use some sort of block or even paper and just account for the thickness of what was used.

[@khusco1180]

Not