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.
lathe post processor issue ( tool offsets not applied from fusion 360 post processor ? )**SOLVED**
Moderator: cnckeith
-
- 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**
- 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.
-
- Posts: 1982
- 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 ? )
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
But from my POV you are way faster for an easy part like this to use Intercon instead of fusion
Regards
Uwe
-
- 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 ? )
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
-
- Posts: 7334
- 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 ? )
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
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
-
- 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 ? )
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.
-
- Posts: 3102
- 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 ? )
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.
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.
Re: lathe post processor issue ( tool offsets not applied from fusion 360 post processor ? )
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.
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.
-
- 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 ? )
Thank you, that helps a lot.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.
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
-
- 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 ? )
Bingo ! thank you! That was it.
Best Regards,
Jake