Post Processor

This forum is for general discussion about Aspire
Post Reply
Barrie123
Posts: 4
Joined: Sun Oct 06, 2019 1:57 am
Model of CNC Machine: ELE1316

Post Processor

Post by Barrie123 »

Is any one able to advise the post processor for the Rotary Toolpath for a Blue Elephant Chinese CNC.
My Model is a 1600x1300x400 ( 1600x 1300 Table and 400 Gantry )
I use a Rich Auto B18 Hand Controller.
Regards
Barrie

User avatar
Rcnewcomb
Vectric Wizard
Posts: 4186
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: Post Processor

Post by Rcnewcomb »

You can take the existing Rich Auto A11 Dsp (mm) post processor, make a copy, and add the two modifications shown in this thread: UCCNC Post Processor for Wrapping
- Randall Newcomb
10 fingers in, 10 fingers out
another good day in the shop

kstrauss
Vectric Craftsman
Posts: 228
Joined: Mon Apr 29, 2013 3:37 am
Model of CNC Machine: Tormach PCNC770
Location: Cobourg, ON, Canada

Re: Post Processor

Post by kstrauss »

There are also some excellent instructions in this thread:
viewtopic.php?f=2&t=35829

User avatar
Rcnewcomb
Vectric Wizard
Posts: 4186
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: Post Processor

Post by Rcnewcomb »

Explaining in a bit more detail.

Post processor files are just text files that guide the Vectric program on how to convert the toolpaths to specific instructions for your machine. If you have a background in older Windows systems they are similar to the INI files that Windows programs used. They can be edited with a text editor such as Notepad, Notepad++, SublimeText, etc.

To find a post processor to modify, open the Vectric program (Aspire or VCarve) and choose:
File/Open Application Data Folder
Screen Shot 2020-10-18 at 12.10.01 PM.png
This window opens. I'm running Windows 10 in Dark mode so your screen may appear slightly different.
OpenApplicationFolder.JPG
Open the PostP folder and you will see a lit of all the available post processor files.
PostPfolder.JPG

in this case we are looking for the Rich Auto post processor. So we scroll until we find it. (You could also use the Search feature of Windows Explorer).
RichAuto.JPG
Use a text editor to look at the file. Notepad defaults to looking for files with a .TXT extension. You will need to change notepad to look at All file types so you can open a file with a .PP extension.
NotepadOpen.JPG
Here is what the top of the file looks like.
NotePPheader.JPG
Before you do anything else, save the current file under a new name!


I'd suggest adding the word WRAP to the file name.
- Randall Newcomb
10 fingers in, 10 fingers out
another good day in the shop

User avatar
Rcnewcomb
Vectric Wizard
Posts: 4186
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: Post Processor

Post by Rcnewcomb »

Editing the File
A step that people sometimes forget is to change the POST_NAME inside the file. Best practices are to keep the name of the file and the POST_NAME the same.

In the earlier step I saved the file as Rich_Auto_A11_Dsp_Wrap_mm.PP
RichAutoNewName.JPG

The POST_NAME line currently shows
POST_NAME = "Rich Auto A11 Dsp (mm) (*.plt)"
I'm going to change it to
POST_NAME = "Rich Auto A11 Dsp WRAP (mm) (*.plt)"


Next we will add the ROTARY_WRAP command. The purpose of the command is to tell the software to translate moves in the X or Y direction to rotary moves. In the example below I've told it to translate X moves into A moves. The software handles the math of converting to a rotational movement.

Code: Select all

POST_NAME = "Rich Auto A11 Dsp WRAP (mm) (*.plt)"

FILE_EXTENSION = "plt"

UNITS = "MM"

ROTARY_WRAP_X = "A"
If your rotary is PERPENDICULAR to the X axis you want ROTARY_WRAP_X
If your rotary is PERPENDICULAR to the Y axis you want ROTARY_WRAP_Y

You can include or omit the minus sign in front of the A depending on the direction you want the rotary to move. (Hint: if your text is coming out backwards try adding or omitting the minus sign). Example: ROTARY_WRAP_X = "-A"

If your setup uses B for the rotary axis then substitute B rather than A. For example: ROTARY_WRAP_X = "B"
If you want the Y-axis moves wrapped rather than the X-axis moves the command would be: ROTARY_WRAP_Y = "A"
- Randall Newcomb
10 fingers in, 10 fingers out
another good day in the shop

User avatar
Rcnewcomb
Vectric Wizard
Posts: 4186
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: Post Processor

Post by Rcnewcomb »

Creating a Rotary Job
When you set up the rotary job be sure to use the correct orientation. Is your rotary axis parallel to the X or Y direction. My setup is parallel Y so I select:
ParallelY.JPG

Create a basic test file with some text. This will help you determine if you need to add or remove a negative sign on the ROTARY line in the post processor.
TestFileRotary.JPG

When you save the toolpaths be sure to select your new post processor.
RichAutoRotaryPostP.JPG

After you have saved the toolpath file use a text editor to look at the output. Below is an example that shows movements in A, Y, and Z

Code: Select all

N0 G0 Z63.500
N1 G0A-233.269 Y172.638 Z57.150
N2 G1A-233.269 Y172.638 Z48.177
N3 G1A-233.269 Y180.806 Z48.177
N4 G1A-135.392 Y180.806 Z48.177
- Randall Newcomb
10 fingers in, 10 fingers out
another good day in the shop

SteveNelson46
Vectric Wizard
Posts: 974
Joined: Wed Jan 04, 2012 2:43 pm
Model of CNC Machine: Camaster Stinger using WinCNC
Location: Tucson, Az.

Re: Post Processor

Post by SteveNelson46 »

Randall,

I like the way you make it look simple.
Steve

rwilkens
Posts: 4
Joined: Thu Feb 06, 2020 2:56 pm
Model of CNC Machine: Legacy

Re: Post Processor

Post by rwilkens »

Rcnewcomb wrote:
Sun Oct 18, 2020 8:49 pm
Explaining in a bit more detail.

Post processor files are just text files that guide the Vectric program on how to convert the toolpaths to specific instructions for your machine. If you have a background in older Windows systems they are similar to the INI files that Windows programs used. They can be edited with a text editor such as Notepad, Notepad++, SublimeText, etc.

To find a post processor to modify, open the Vectric program (Aspire or VCarve) and choose:
File/Open Application Data Folder
Screen Shot 2020-10-18 at 12.10.01 PM.png

This window opens. I'm running Windows 10 in Dark mode so your screen may appear slightly different.
OpenApplicationFolder.JPG

Open the PostP folder and you will see a lit of all the available post processor files.
PostPfolder.JPG


in this case we are looking for the Rich Auto post processor. So we scroll until we find it. (You could also use the Search feature of Windows Explorer).
RichAuto.JPG

Use a text editor to look at the file. Notepad defaults to looking for files with a .TXT extension. You will need to change notepad to look at All file types so you can open a file with a .PP extension.
NotepadOpen.JPG

Here is what the top of the file looks like.
NotePPheader.JPG

Before you do anything else, save the current file under a new name!


I'd suggest adding the word WRAP to the file name.
My machine cuts a mirrored image. I assume I need to add a code to the mach3 processor to tell it that x=-x and y=-y.
What code statement would I have to add to correct that condition?

rwilkens
Posts: 4
Joined: Thu Feb 06, 2020 2:56 pm
Model of CNC Machine: Legacy

Re: Post Processor

Post by rwilkens »

My machine cuts a mirrored image. I assume I need to add a code to the mach3 processor to tell it that x=-x and y=-y.
What code statement would I have to add to correct that condition?

User avatar
Rcnewcomb
Vectric Wizard
Posts: 4186
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: Post Processor

Post by Rcnewcomb »

My machine cuts a mirrored image.
In just rotary, or flat as well?
Is it mirrored right to left, upside down, or both?
- Randall Newcomb
10 fingers in, 10 fingers out
another good day in the shop

rwilkens
Posts: 4
Joined: Thu Feb 06, 2020 2:56 pm
Model of CNC Machine: Legacy

Re: Post Processor

Post by rwilkens »

Using flat stock. New machine. Mirrored to left.

rwilkens
Posts: 4
Joined: Thu Feb 06, 2020 2:56 pm
Model of CNC Machine: Legacy

Re: Post Processor

Post by rwilkens »

Aspire and mach3 showed image correctly but cut mirrored to left. New Chinese machine which I set up with the X axis along the length of the bed and Y axis along width. Chinese machines set up opposite. If I manually enter X5,Y5 machine moves correctly. UC100 board. Purchased 3x4 floor machine for my nephew who lives in a different state and had to do the setup over the phone. Read the rotary post processor procedure and was hopeful I could correct the problem using that procedure.

User avatar
Rcnewcomb
Vectric Wizard
Posts: 4186
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: Post Processor

Post by Rcnewcomb »

You may be able to change this in Mach3. I'll defer to the Mach experts on this. (I'm a ShopBot and WinCNC guy.)
- Randall Newcomb
10 fingers in, 10 fingers out
another good day in the shop

User avatar
Rcnewcomb
Vectric Wizard
Posts: 4186
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: Post Processor

Post by Rcnewcomb »

You may want to search and/or ask on the Mach Support Forum

See this thread: Mirrored Milling(backwards text) Mach 3
- Randall Newcomb
10 fingers in, 10 fingers out
another good day in the shop

Post Reply