Changing Post Processor for Side Drill

This forum is for requests and queries about machine tool support for Vectric Products
Post Reply
User avatar
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

Post by BenjaminwithCNC »

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?
Attachments
Syntec_arc_mm.pp
(4.24 KiB) Downloaded 150 times

User avatar
adze_cnc
Vectric Wizard
Posts: 4303
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

Post by adze_cnc »

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.

User avatar
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

Post by BenjaminwithCNC »

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

User avatar
Leo
Vectric Wizard
Posts: 4080
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

Post by Leo »

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.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

User avatar
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

Post by BenjaminwithCNC »

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

User avatar
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

Post by BenjaminwithCNC »

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.

User avatar
SteveNelson46
Vectric Wizard
Posts: 2275
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

Post by SteveNelson46 »

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

User avatar
adze_cnc
Vectric Wizard
Posts: 4303
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

Post by adze_cnc »

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:

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]
to

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]
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...

User avatar
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

Post by BenjaminwithCNC »

Thank you very much for that piece of Information.

This helped a lot.

Post Reply