lathe post processor issue ( tool offsets not applied from fusion 360 post processor ? )**SOLVED**

All things related to the Centroid Acorn CNC Controller

Moderator: cnckeith

Post Reply
cut2cut
Posts: 74
Joined: Sat Dec 23, 2017 3:02 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D26950ABAB-1221170383
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

lathe post processor issue ( tool offsets not applied from fusion 360 post processor ? )**SOLVED**

Post by cut2cut »

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.
Attachments
report_38D26950ABAB-1221170383_2021-10-15_12-22-26.zip
(616.99 KiB) Downloaded 268 times
3000.cnc
(3.36 KiB) Downloaded 283 times
Last edited by cut2cut on Mon Oct 18, 2021 11:57 pm, edited 1 time in total.
suntravel
Posts: 1967
Joined: Thu Sep 23, 2021 3:49 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 6433DB0446C1-08115074
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Germany

Re: lathe post processor issue ( tool offsets not applied from fusion 360 post processor ? )

Post by suntravel »

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
cut2cut
Posts: 74
Joined: Sat Dec 23, 2017 3:02 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D26950ABAB-1221170383
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: lathe post processor issue ( tool offsets not applied from fusion 360 post processor ? )

Post by cut2cut »

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
cnckeith
Posts: 7164
Joined: Wed Mar 03, 2010 4:23 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: Yes
CNC Control System Serial Number: none
DC3IOB: Yes
CNC11: Yes
CPU10 or CPU7: Yes
Contact:

Re: lathe post processor issue ( tool offsets not applied from fusion 360 post processor ? )

Post by cnckeith »

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.
Need support? READ THIS POST first. http://centroidcncforum.com/viewtopic.php?f=60&t=1043
All Acorn Documentation is located here: viewtopic.php?f=60&t=3397
Answers to common questions: viewforum.php?f=63
and here viewforum.php?f=61
Gear we use but don't sell. https://www.centroidcnc.com/centroid_di ... _gear.html
vw_chuck
Posts: 194
Joined: Sun Sep 20, 2020 7:34 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 0035FF8FEB5F-0708203490
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No

Re: lathe post processor issue ( tool offsets not applied from fusion 360 post processor ? )

Post by vw_chuck »

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.
tblough
Posts: 3072
Joined: Tue Mar 22, 2016 10:03 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: Yes
CNC Control System Serial Number: 100505
100327
102696
103432
7804732B977B-0624192192
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Boston, MA
Contact:

Re: lathe post processor issue ( tool offsets not applied from fusion 360 post processor ? )

Post by tblough »

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.
Cheers,

Tom
Confidence is the feeling you have before you fully understand the situation.
I have CDO. It's like OCD, but the letters are where they should be.
cncsnw
Posts: 3763
Joined: Wed Mar 24, 2010 5:48 pm

Re: lathe post processor issue ( tool offsets not applied from fusion 360 post processor ? )

Post by cncsnw »

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.
cut2cut
Posts: 74
Joined: Sat Dec 23, 2017 3:02 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D26950ABAB-1221170383
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: lathe post processor issue ( tool offsets not applied from fusion 360 post processor ? )

Post by cut2cut »

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
cut2cut
Posts: 74
Joined: Sat Dec 23, 2017 3:02 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D26950ABAB-1221170383
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: lathe post processor issue ( tool offsets not applied from fusion 360 post processor ? )

Post by cut2cut »

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
Attachments
Screen Shot 2021-10-18 at 8.56.09 PM.jpg
Screen Shot 2021-10-18 at 6.08.29 PM.jpg
Post Reply