Where to place the post processor in Aspire or V-Carve Pro

[Mick Martin]

Do not use the post processor the comes with Aspire or V-Carve Pro, CAMaster and Wincnc have written specific post processors for CAMaster machines.

Either download the post processor for your specific machine off the forum or contact one of the Knights, Moderators or CAMaster.

- Next start Aspire or V-Carve Pro.



- Click on 'file' in the upper left hand corner.
- In the drop-down menu, click on 'Open Application Data Folder'.



- Double click on the PostP folder.



- Create a new folder called un-used PP.
- MOVE all the files (not the folders) into your new folder.
- Now copy the post processor you saved into the original PostP folder (it should be the only file) there will be folders.



- Close all the folders.
- Restart Aspire or V-Carve Pro.

[Mick Martin]

Continued

Check to see if the post processor is installed correctly

- Start Aspire or V-Carve Pro.
- Click on create new file.
- Enter width 5, Height 5, Thickness 1, Z0 wherever you want (these are just values not important)
- Click OK.
- Click on the toolpath tab icon.



- Click on the save toolpath icon.



See the section called post processor, if you click on the pull down menu you will only see one post processor unless you have a recoil in that case you will have two post processors.



I hope this helps ...... it is quicker to install the post processor than me making this message.

[Mark Johnston]

Hi Mick,

I noticed when I updated to Aspire 4.0 that Vectric has 6 CAMaster post processors included with their software now. I assumed that CAMaster provided them, of course I know what it is to assume.

Just to clarify should we or at least the new guys use these or continue to get them from CAMaster?

Nice write up by the way.

Mark

[Mick Martin]

Just to clarify should we or at least the new guys use these or continue to get them from CAMaster?

Mark

Mark,
Good point I would use the post processor designed by CAMaster and Wincnc, I just viewed the post processor that Vectric provides with it's software and it's not the current version, there have been some changes made to the CAMaster version.

F[FC] XY"
F[FP] Z"

Feed rates for XYZ are not included in the Aspire post processor version

[sscooter]

Mick
I have used the PP's from Aspire 3.5,4.0 and have no problems that I know of. If there are better ones here on the forum, were do we find them? I would need the ones for a Stinger1, Stinger1 FTC, and Stinger1 W/Recoil.

Thanks Again

[Mick Martin]

Mick
I have used the PP's from Aspire 3.5,4.0 and have no problems that I know of. If there are better ones here on the forum, were do we find them? I would need the ones for a Stinger1, Stinger1 FTC, and Stinger1 W/Recoil.

Thanks Again

Here you go Chuck, these post processors are for an FTC machine, do you have the auto on/off relay? Keep you old post processor and add these.

[sscooter]

Yes I have spindle on by G-code, I that's the main reason I ordered the FTC option. Now that I can use the FTC since fixing my INI file its pretty cool too!

[TErb2012]

Can someone please send me the PP's please.

[Gary Campbell]

Terry, et al...
CAMaster posts are on the forum for Download in the Owners Only section: CAMheads CNC Router Forum By: CAMaster CNC > CAMaster Machines > CAMaster Owners Only > CAMaster Tech > CAMaster Post > Vectric Post

[TErb2012]

What now???

Good afternoon all, so I read this post thoroughly and twice for that fact. Much like "sscooter" I've used PP from 3.5 and 4 with no problem. However since then I followed the recommendations from many on this forum and updated my PP with the ones listed in the users Forum.

Following the directions carefully I placed the PP in the exact location identified in the previous post. I recently prepared a project to be machined and saved the toolpaths with the new PP and encountered the following error when I tried to run them on my Stinger 1. While in the WINCNC menu I can no longer use the view button without encountering the same error message depicted in the attached pic. I wanted to double check myself to see if I did something wrong and loaded one of my toolpaths with the older PP and everything worked fine.

I can easily load the PP that came with Aspire 4 however, if these are in fact the correct/most updated PP I should be using I'd prefer to use them. Any help will be greatly appreciated.


Here are the PP I downloaded for my Stinger 1 equipped with a Recoil.
CAMaster_Arcs_inch
CAMaster_Recoil_X2A_IN
CAMaster_Stinger_IN

[Mick Martin]

Terry,

You do not have an FTC .... correct?
Do you have an auto on/off (via G-Code) for your router?
The way to test it is to start your CNC and computer using the normal start up process. once the CNC is Initialized do the following:
- Jog the router anywhere on the spoilboard
- Raise Z up 2" or more off the spoilboard (with or without a router bit installed)
- In Wincnc in the command box type M3 then press enter - if you have an auto on/off relay it will start the router
- Next in Wincnc type M5 them press enter - this will turn off the router.

Let me know what happens.

[TErb2012]

That is correct, I don not have an FTC.
I'm presuming the answer to the On/Off is yes for my spindle.
Did as you asked the command M3 turned the spindle on and M5 turned it off.

Standing by for further guidance/instructions.

Thank you

[Mick Martin]

Terry,

Could you post the first 20 lines of your tap file

[TErb2012]

As requested:

G0Z0.8000
G0X0.0000Y0.0000
T1
SS9000
M3
G0X7.6095Y8.4445Z0.8000
G0Z0.2000
G1Z0.0000F30
G1X7.6233Y8.4297F100
G1X7.6768Y8.4898
G1X7.6414Y8.5690
G1X7.6095Y8.4445
G1X7.5540Y8.4306
G1X7.6244Y8.3547
G1X7.7359Y8.4806
G1X7.6275Y8.7302
G1X7.5540Y8.4306
G1X7.4983Y8.4166
G1X7.6255Y8.2790
G1X7.7930Y8.4690

[Mick Martin]

As requested:

G0Z0.8000
G0X0.0000Y0.0000
T1
SS9000
M3
G0X7.6095Y8.4445Z0.8000
G0Z0.2000
G1Z0.0000F30
G1X7.6233Y8.4297F100
G1X7.6768Y8.4898
G1X7.6414Y8.5690
G1X7.6095Y8.4445
G1X7.5540Y8.4306
G1X7.6244Y8.3547
G1X7.7359Y8.4806
G1X7.6275Y8.7302
G1X7.5540Y8.4306
G1X7.4983Y8.4166
G1X7.6255Y8.2790
G1X7.7930Y8.4690

Terry,

You don't have speed control on your router?
Here is your problem SS9000

Open your post processor CAMaster_Stinger_IN and delete the line in red below, save your post processor and then re-save your design files.

A quick option is to open your tap file and delete the line SS9000

begin HEADER

"[N] [91][TP_FILENAME][93]"
"[N] [91][TIME], [DATE][93]"
"[N] "
"[N] [91]MATERIAL size: [XLENGTH][34] x [YLENGTH][34] x [ZLENGTH][34][93]"
"[N] "
"[N] [91][TOOLNAME][93]"
"[N] "
"[N] G90 [91]ABSOLUTE MODE[93]"
"[N] "
"[N] M5 [91]SPINDLE OFF[93]"
"[N] G53 Z0 [91]LIFT Z TO TOP[93]"
"[N] "
"[N] [S] [91] SET SPINDLE SPEED RPM [93]"
"[N] M3 [91]SPINDLE ON[93]"
"[N] "
"[N] G53 Z0 [91]LIFT Z TO TOP[93]"
"[N] "
"[N] F[FC] XY [91]SET FEEDRATE FOR X AND Y[93]"
"[N] F[FP] Z [91]SET FEEDRATE FOR Z[93]"
"[N] "

You should be good to go after that