Good Day to everyone!
I'm trying to get my Side Milling Unit to work, it is Syntec 6MB Controlled. What I'm trying to do, is change the Post Processor so that it will change the X+ into Z-. and Z- into X+.
how can i do that? Anyone have a clue?
Changing Post Processor for Side Drill
- BenjaminwithCNC
- Posts: 29
- Joined: Thu Feb 25, 2021 8:22 am
- Model of CNC Machine: Danibrum 1325 ATC Rotary 4x1
Changing Post Processor for Side Drill
- Attachments
-
- Syntec_arc_mm.pp
- (4.24 KiB) Downloaded 150 times
- adze_cnc
- Vectric Wizard
- Posts: 4380
- Joined: Sat Jul 27, 2013 10:08 pm
- Model of CNC Machine: AXYZ 4008
- Location: Vancouver, BC, Canada
Re: Changing Post Processor for Side Drill
Rather than trying to remap the X & Z axes via the post-processor how about rotating the cutting plane instead: https://www.cnc.com/g17-g18-g19-plane-selection-gcodes/
The conflict with remapping the axes is that you, in a sense, want "Z" to be both positive and negative depending on whether it's X mapped to Z or Z mapped to X.
The conflict with remapping the axes is that you, in a sense, want "Z" to be both positive and negative depending on whether it's X mapped to Z or Z mapped to X.
- BenjaminwithCNC
- Posts: 29
- Joined: Thu Feb 25, 2021 8:22 am
- Model of CNC Machine: Danibrum 1325 ATC Rotary 4x1
Re: Changing Post Processor for Side Drill
Thank you a lot. I looked into it, now here is my question, if the Side milling unit is on the left side of my material and i want to mill a rectangle on the left side, where do i place the rectangle so it mills it right?
Would that mean,to use the Cut depth for the positioning and the X position as a Cut depth?
I'm confused
Would that mean,to use the Cut depth for the positioning and the X position as a Cut depth?
I'm confused
- Leo
- Vectric Wizard
- Posts: 4092
- Joined: Sat Jul 14, 2007 3:02 am
- Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
- Location: East Freetown, Ma.
- Contact:
Re: Changing Post Processor for Side Drill
Plane selection is more about G2 G3 arc cutting. If I were going to Gcode the side drilling I would just use the X oy Y commands
In vectric, I would do something with a profile ON a line tools.
In vectric, I would do something with a profile ON a line tools.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC
- BenjaminwithCNC
- Posts: 29
- Joined: Thu Feb 25, 2021 8:22 am
- Model of CNC Machine: Danibrum 1325 ATC Rotary 4x1
Re: Changing Post Processor for Side Drill
I think i'll go back to the initial Question about Post Processor, that way i can draw it with Vectric, only thing, how to change X to Z and Z to X.
i searched about the Wrap Function but it uses this one: ROTARY_WRAP_X = "-A", which is explicitly Rotary. Manuals don't show anything.
Thank you for your time.
Benjamin
i searched about the Wrap Function but it uses this one: ROTARY_WRAP_X = "-A", which is explicitly Rotary. Manuals don't show anything.
Thank you for your time.
Benjamin
- BenjaminwithCNC
- Posts: 29
- Joined: Thu Feb 25, 2021 8:22 am
- Model of CNC Machine: Danibrum 1325 ATC Rotary 4x1
Re: Changing Post Processor for Side Drill
Good morning,
I tried using this:
SUBSTITUTE = "O1 S1 O2 S2 On Sn"
but it don't think i can use it only i a Segment. So that i could move the Side unit to X-10 position and then start my milling.
I tried using this:
SUBSTITUTE = "O1 S1 O2 S2 On Sn"
but it don't think i can use it only i a Segment. So that i could move the Side unit to X-10 position and then start my milling.
- SteveNelson46
- Vectric Wizard
- Posts: 2310
- Joined: Wed Jan 04, 2012 2:43 pm
- Model of CNC Machine: Camaster Stinger 1
- Location: Tucson, Az.
Re: Changing Post Processor for Side Drill
Generally speaking, post processors are controller/machine specific and are usually written by machine or controller manufacturers and provided to Vectric by request. Many here on the forum are good with writing g-code but few are familiar with your machine or controller. I think your question would be best answered by your machine or controller manufacturer.
Steve
- adze_cnc
- Vectric Wizard
- Posts: 4380
- Joined: Sat Jul 27, 2013 10:08 pm
- Model of CNC Machine: AXYZ 4008
- Location: Vancouver, BC, Canada
Re: Changing Post Processor for Side Drill
Sorry about the wrong lead on remapping the XYZ plane using Gxx commands. I knew such a feature existed but I didn't realize it was only for arcs.
I still think re-orienting the XYZ plane on the machine is the way to go and you might just have found something. But as Steve mentioned we don't know your machine so can't really verify it for you.
Back to your question about altering the post-processor file (and part of me doesn't even want to post this information):
In the following I'm using lines from my post-processor. You'd have to find similar ones in yours. I guess the easiest way to do that is changing the lines:
to
This should work but I haven't verified it. Also, it would be incumbent on you to set up your job so that the remapped X and Z axes go in the right positive and negative directions. Also, there might be other variables that would need swapping.
Also, if your post processor uses: ???_ARC_MOVE entries you'd probably want to comment them out as I'm not sure how they would react to the remapped axes without a remapping of the XYZ plane...
I still think re-orienting the XYZ plane on the machine is the way to go and you might just have found something. But as Steve mentioned we don't know your machine so can't really verify it for you.
Back to your question about altering the post-processor file (and part of me doesn't even want to post this information):
In the following I'm using lines from my post-processor. You'd have to find similar ones in yours. I guess the easiest way to do that is changing the lines:
Code: Select all
VAR X_POSITION = [X|C|X|1.4]
VAR Z_POSITION = [Z|C|Z|1.4]
VAR X_HOME_POSITION = [XH|C|X|1.4]
VAR Z_HOME_POSITION = [ZH|C|Z|1.4]
VAR SAFE_Z_HEIGHT = [SAFEZ|A|Z|1.4]
Code: Select all
VAR X_POSITION = [Z|C|X|1.4]
VAR Z_POSITION = [X|C|Z|1.4]
VAR X_HOME_POSITION = [ZH|C|X|1.4]
VAR Z_HOME_POSITION = [XH|C|Z|1.4]
VAR SAFE_Z_HEIGHT = [SAFEZ|A|X|1.4]
Also, if your post processor uses: ???_ARC_MOVE entries you'd probably want to comment them out as I'm not sure how they would react to the remapped axes without a remapping of the XYZ plane...
- BenjaminwithCNC
- Posts: 29
- Joined: Thu Feb 25, 2021 8:22 am
- Model of CNC Machine: Danibrum 1325 ATC Rotary 4x1
Re: Changing Post Processor for Side Drill
Thank you very much for that piece of Information.
This helped a lot.
This helped a lot.