Centroid Community CNC Support Forum

Hi,

I'm fairly new to centroid lathe tool offsets so I thought my issue outputting lathe cam from fusion 360, but *not* applying tool offsets, was that I didn't understand how to create offsets properly within Centroid. However, I used intercon yesterday to create a multi tool program and it worked fine ( tool offsets were applied perfectly ) . So I know the issue is either with the centroid lathe post processor, or with Fusion 360 itself ( or user error = me ). I'm not conversant with Gcode, so I'm including it in my post. I'm hoping someone can suggest a setting in Fusion 360 that I'm overlooking, or perhaps its a known issue with the lathe post processor ?

Jake

report file enclosed as well as an example of gcode that isn't using the tool offsets when changing tools.

What is missing ist the H(toolnumber) for the tools to let Acorn know the offsets.

But from my POV you are way faster for an easy part like this to use Intercon instead of fusion

Regards

Uwe

suntravel wrote: ↑Sun Oct 17, 2021 3:47 pm What is missing ist the H(toolnumber) for the tools to let Acorn know the offsets.

But from my POV you are way faster for an easy part like this to use Intercon instead of fusion

Regards

Uwe

So, should I poke around Fusion 360 to see if it will output the H(toolnumber) by clicking the right check box ? Or is it more likely a post processor issue ?

Yes, intercon is pretty cool, but for this post I used a very simple operation just to keep the size down for this example.
Thanks!

Jake

often i will use intercon generated g code to debug cad/cam generated g code by comparing them as i know the intercon g code will run on cnc12, so looking at intercon generated g code helps me debug the post processor output.

You need to put the tool number and offset number in the tool library for each tool. If you edit the tool under the general tab it has Number and Comp Offset. Also check the manual tool change if you are manually changing tools.

I don't know about F360 but in SolidCAM, you enter the tool offset numbers for length and diameter in the project tool table, but you ALSO have to check "apply diameter compensation to finish passes" for each operation that you want to use compensation on. Possibly F360 has something along these lines as well.

Lathe tool offsets do not use "H__".

Instead, in lathe G codes, the second two digits of the tool number specifies the offsets to use.

For example:
T1200 ; load tool #12, but use no offsets
T1212 ; load tool #12, and activate offsets #12

The problem in your program is that for each tool change, while the tool number is there in the first two digits, the offset in the second two digits was left at 00. Thus you get no offsets applied.

cncsnw wrote: ↑Mon Oct 18, 2021 3:46 pm Lathe tool offsets do not use "H__".

Instead, in lathe G codes, the second two digits of the tool number specifies the offsets to use.

For example:
T1200 ; load tool #12, but use no offsets
T1212 ; load tool #12, and activate offsets #12

The problem in your program is that for each tool change, while the tool number is there in the first two digits, the offset in the second two digits was left at 00. Thus you get no offsets applied.

Thank you, that helps a lot.

I suppose my only option is to search and “fix” the Toolchange gcode by adding the offset value by hand (manually) until i find the reason the post processor OR Fusion 360 isnt outputting the offset data.

Best,
Jake

vw_chuck wrote: ↑Mon Oct 18, 2021 2:47 pm You need to put the tool number and offset number in the tool library for each tool. If you edit the tool under the general tab it has Number and Comp Offset. Also check the manual tool change if you are manually changing tools.

Bingo ! thank you! That was it.

Best Regards,

Jake