Set Acorn So It Homes In Z then X Direction. Not the two at once?

All things related to the Centroid Acorn CNC Controller

Moderator: cnckeith

Post Reply
ChrisMe
Posts: 40
Joined: Sat Feb 27, 2021 7:38 am
Acorn CNC Controller: No
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Set Acorn So It Homes In Z then X Direction. Not the two at once?

Post by ChrisMe »

How do I set the lathe machine home so it moves in the Z then the X axis instead of both at the same time? Currently when it's time to change tools the tool is crashing into the part on it's way to the home position.
tblough
Posts: 1706
Joined: Tue Mar 22, 2016 10:03 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: Yes
MPU11 & GPIO4D -w/ 3rd Party Drives: Yes
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 100505
100327
102696
103432
7804732B977B-0624192192
Location: Boston, MA
Contact:

Re: Set Acorn So It Homes In Z then X Direction. Not the two at once?

Post by tblough »

Are you using Intercon or some other program to generate your g-code? You need to add in the correct moves to clear your part before calling a tool change.
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.
ChrisMe
Posts: 40
Joined: Sat Feb 27, 2021 7:38 am
Acorn CNC Controller: No
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Re: Set Acorn So It Homes In Z then X Direction. Not the two at once?

Post by ChrisMe »

I'm just using the free Acorn CNC12 Lathe software. Is it worth while setting the tool up to do a finishing pass ending at the home point so it all works OK?
cncsnw
Posts: 2278
Joined: Wed Mar 24, 2010 5:48 pm

Re: Set Acorn So It Homes In Z then X Direction. Not the two at once?

Post by cncsnw »

Usually, a lathe is set to home to the X+ limit and Z+ limit.
We do not know which direction your machine homes in, because you have not posted a Report here.

Usually, if you use Intercon in CNC12 to generate your programs, tool changes take place at the G28 position.

Usually, the G28 position is at machine X0 Z0 (i.e. at the machine home position).
We do not know where your G28 position is set, because you have not posted a Report here.

With most part programs, if the tool has just finished a cut, it is in a location where a straight move to a G28 position that is at the X+ and Z+ limits will not hit the part on the way.
We do not know if that is the case with your part program, because you have not posted a copy of your part program here.

In those rare cases where that is not true (e.g. turning OD features behind a raised flange/wall, or working inside a bore without a retract to the free end of the part), you should add a Rapid move to get the tool from the end of the cut, to a place where it is safe to move to home (e.g. to an X diameter larger than the largest feature on the part, and/or to a Z position clear of the free end).
vw_chuck
Posts: 104
Joined: Sun Sep 20, 2020 7:34 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 0035FF8FEB5F-0708203490

Re: Set Acorn So It Homes In Z then X Direction. Not the two at once?

Post by vw_chuck »

It is in your post processor.
If you are using Fusion 360 when you hit post process it is in the box in the corner. Under safe retract style you can tell it to go X then Y for your G28 move.
The G28 is your tool change position.
Also you need to set a G28 position for each part so that it doesn't hit the part on retract.
vw_chuck
Posts: 104
Joined: Sun Sep 20, 2020 7:34 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 0035FF8FEB5F-0708203490

Re: Set Acorn So It Homes In Z then X Direction. Not the two at once?

Post by vw_chuck »

Oh also make sure that you are using the latest centroid lathe post processor as the old one had issues in the G28 department.
ChrisMe
Posts: 40
Joined: Sat Feb 27, 2021 7:38 am
Acorn CNC Controller: No
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Re: Set Acorn So It Homes In Z then X Direction. Not the two at once?

Post by ChrisMe »

vw_chuck wrote: Mon Oct 11, 2021 2:36 pm It is in your post processor.
If you are using Fusion 360 when you hit post process it is in the box in the corner. Under safe retract style you can tell it to go X then Y for your G28 move.
The G28 is your tool change position.
Also you need to set a G28 position for each part so that it doesn't hit the part on retract.
Thank you. I'm not using any add ons just the free CNC12 Lathe. How do I do the G28 in centroids software? Thanks.
vw_chuck
Posts: 104
Joined: Sun Sep 20, 2020 7:34 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 0035FF8FEB5F-0708203490

Re: Set Acorn So It Homes In Z then X Direction. Not the two at once?

Post by vw_chuck »

Oh the G28 position is in Return tab under Part tab. As far as retract style I have no idea how you make the Y move first and then X in the Centroid software. Not sure you can.
If your G28 position is behind your part you should never run into issues of it hitting the part on retract. Just set your G28 position behind the part (Z positive) and it should work just fine.
I have asked for a one button g28 reset position on the control panel but apparently that is impossible for them to do since it need memory to do it.....so us lathe guys have to reset the cumbersome way unfortunately.
ChrisMe
Posts: 40
Joined: Sat Feb 27, 2021 7:38 am
Acorn CNC Controller: No
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Re: Set Acorn So It Homes In Z then X Direction. Not the two at once?

Post by ChrisMe »

vw_chuck wrote: Mon Oct 11, 2021 3:22 pm Oh the G28 position is in Return tab under Part tab. As far as retract style I have no idea how you make the Y move first and then X in the Centroid software. Not sure you can.
If your G28 position is behind your part you should never run into issues of it hitting the part on retract. Just set your G28 position behind the part (Z positive) and it should work just fine.
I have asked for a one button g28 reset position on the control panel but apparently that is impossible for them to do since it need memory to do it.....so us lathe guys have to reset the cumbersome way unfortunately.
This is good to know. I was making a small part and the G28 position was just behind the finished part but as the tool went in a straight line it hit the part. I'll just set the home to behind the Z and X axis which is a shame as having the tool where it was, was a good way to make sure I had the stock sitting out as little as possible.
tblough
Posts: 1706
Joined: Tue Mar 22, 2016 10:03 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: Yes
MPU11 & GPIO4D -w/ 3rd Party Drives: Yes
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 100505
100327
102696
103432
7804732B977B-0624192192
Location: Boston, MA
Contact:

Re: Set Acorn So It Homes In Z then X Direction. Not the two at once?

Post by tblough »

You should set your return point before starting Intercon. Then the return to home moves while graphing will show correctly.

Graphing inside Intercon will show the complete tool path starting from the current tool position, and you can use the feed override knob to control the speed it graphs. If any of the RED rapid moves cross the yellow feedrate moves, then you possibly have a problem, and should correct it by adding intermediate moves to direct the tool clear of the part.

Intercon programs start from the current tool position, moves directly to the return point for the first tool change, then executes the program moves. If you have multiple tools, Intercon will move to the return point directly from where the previous move ended. When the program finishes, Intercon will move directly to the return position.

So, it is up to the programmer (YOU) to make sure the previous move before a tool change clears the part. You may have to enter a feedrate or rapid move in either X or Z before the toolchange to accomplish this.
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.
Post Reply