CAMheads CNC Router Forum By: CAMaster CNC

Go Back   CAMheads CNC Router Forum By: CAMaster CNC > Software > Vectric - Aspire

Reply
 
Thread Tools Display Modes
  #11  
Old 04-10-2021, 06:07 PM
Jim Becker Jim Becker is offline
ADMINISTRATOR
 
Join Date: Jan 2018
Location: SE PA
Posts: 2,045
Default

ATC and FTC are both affected and yes, folks only doing single tool toolpath files don't have to worry about it. It's good you were able to create that macro, however, for folks who want to automate the renumbering.
__________________
---
Jim Becker

SR-44 (2018), 1.7kw spindle, Performance Premium, USB, Keypad, T-Slot table (y-axis configuration), WinCNC, VCarve Pro upgraded to Aspire

Non CNC stuff...

SCM/Minimax - slider/JP/BS
Festool "a good collection"
Stubby - lathe
Oneida Cyclone
more...

Retired from full time work in the telecom industry 9/2017
Commission work for equestrian tack storage and other custom furniture and cabinetry
Located Bucks County PA
Reply With Quote
  #12  
Old 04-10-2021, 07:09 PM
DVE2000 DVE2000 is offline
CAMaster Owner
 
Join Date: Aug 2018
Posts: 555
Default

Youíre not getting it. If you have an ATC, you want tool numbers to never change. If tool 1 is your half inch spiral up cut, thatís the number it has to be. It would be pretty idiotic to run the tool renumber gadget.

However, if you have an FTC, and you have to MANUALLY change bits, the tool number is irrelevant. T<number> is needed to run the tool change macro. The post could ALWAYS use T1 to do a tool change (for every tool change), as long as the pause message tells you the ACTUAL bit that is required to be inserted. So you run the tool renumber gadget and you can STILL use the tool change post to create the tap file. With different tool paths requiring different tools.

Thatís why I modified my post to use [TOOLNAME] instead of [T] (which is the number) as shown in that thread. Repeated here:
" T[T] [91] GET TOOL [TOOLNAME] [93]"
__________________
Gary
2018 Stinger II SR-44, 1.7kW Spindle, Performance Premium, Recoil, Gantry Lift, Cyclone
Fusion 360
Aspire
Reply With Quote
  #13  
Old 04-10-2021, 07:45 PM
Jim Becker Jim Becker is offline
ADMINISTRATOR
 
Join Date: Jan 2018
Location: SE PA
Posts: 2,045
Default

My point was that for ATC and FTC users, in the factory supplied software setup, tool numbers are limited to 0-9 in a multi-tool file. You are absolutely correct that one would never want the numbers to change for an ATC as well as about the fact that there are ways to work around things. You have dived into really well! Initially, at least, most users are not savvy enough to incorporate those workarounds...or even know about them, however. That sometimes creates a situation like with the OP where that tool number got missed through a chunk of the troubleshooting. I am glad, however, that you've detailed the ways to handle this as folks get more confident and knowledgeable.
__________________
---
Jim Becker

SR-44 (2018), 1.7kw spindle, Performance Premium, USB, Keypad, T-Slot table (y-axis configuration), WinCNC, VCarve Pro upgraded to Aspire

Non CNC stuff...

SCM/Minimax - slider/JP/BS
Festool "a good collection"
Stubby - lathe
Oneida Cyclone
more...

Retired from full time work in the telecom industry 9/2017
Commission work for equestrian tack storage and other custom furniture and cabinetry
Located Bucks County PA
Reply With Quote
  #14  
Old 04-11-2021, 02:42 PM
SteveNelson46 SteveNelson46 is offline
CAMaster Owner
 
Join Date: Oct 2018
Location: Tucson, Arizona
Posts: 227
Default

Gary,

I haven't followed the logic flow of your post processor so this may be a dumb question. I have a Stinger 1 with the FTC enabled and often use the same tool for different toolpaths by grouping them together in the tool path list and saving as one file. As long as the tool numbers are the same the FTC will not prompt for a tool change. If the tool numbers are different the FTC will handle them as separate toolpaths. Can your modification handle that?
__________________
Steve
__________________
Camaster Stinger 1 with Recoil (2019)
FTC
1hp Spindle
Laser crosshair
Wireless Pendant
Aspire 10.5

Last edited by SteveNelson46; 04-11-2021 at 02:45 PM.
Reply With Quote
  #15  
Old 04-11-2021, 03:29 PM
DVE2000 DVE2000 is offline
CAMaster Owner
 
Join Date: Aug 2018
Posts: 555
Default

Yes. Vectric decides whether a tool change set of commands is required or not. So if toolpaths using the same tool number are together, no change commands will be inserted into the tap file between them. If the toolpaths have tools with different numbers, you'll get a set of change commands being inserted where appropriate.

This is what you have in the original CAMaster tool change post (in two places):
" T[T] [91] GET TOOL NUMBER [T] [93]"
" [91][TOOLNAME][93]

I haven't used this one in a long time, but the T command calls the macro that lifts Z to the top, moves to the tool change position and does the pause, and then the measure, etc. If I'm recalling correctly, you'll only see the tool name after you've already changed the tool. But I could be wrong about that.

I said I don't care what the tool number actually is, so my post has this in two places:
" T[T] [91] GET TOOL [TOOLNAME] [93]"

So the number is still used for the T command, but the message actually tells me the tool name too.

To be perfectly honest, my post is actually a bit more advanced than that. And my G37.MAC had to be modified to support it:
" G53 x24 Y8"
" [91] REMOVE DUST BOOT AND"
" [91] CHANGE TO '[TOOLNAME]' BIT"
" [91] FOR TOOLPATH '[TOOLPATH_NAME]'"
" [91]THEN PRESS ENTER [93]"
" G4"
" [91] [TOOLPATH_NAME] [93]"
" T[T] [91] GET TOOL [TOOLNAME] [93]"
" [TOOL_NOTES]"

I've, uh, removed the "remove dust boot" message and the G4 (pause) in G37.MAC. Because I now get a message giving me the toolpath AND the tool name when I change bits. So the machine waits for me to change bits with this useful info up on the screen.

And if I really want to insert custom g-code after a bit change, I can put it in the tool notes of the tool in Aspire. Have to be careful though - If it's really a comment and not g-code, it has to start with a square bracket [. Gary Campbell gave a hint for that somewhere on these forums. That man is too smart for his own good! :P
__________________
Gary
2018 Stinger II SR-44, 1.7kW Spindle, Performance Premium, Recoil, Gantry Lift, Cyclone
Fusion 360
Aspire
Reply With Quote
  #16  
Old 04-11-2021, 03:39 PM
DVE2000 DVE2000 is offline
CAMaster Owner
 
Join Date: Aug 2018
Posts: 555
Default

Oh, and the way the gadget works is pretty simple. It uses the name of the tool for number assignment. So if you had 5 toolpaths, with 5 different tools each with the same name (say 1/2" upcut spiral) but with each having a different number, after the script runs, each tool will have the same number because the names are the same. Because that generally means the same tool is needed. If you really want different numbers and want to force tool changes, you can just rename the bit slightly differently in the toolpaths (say 1/2" upcut spiral long). If you did that with one of the toolpaths in my example, you'd end up with 2 tools, and with tool changes as appropriate.
__________________
Gary
2018 Stinger II SR-44, 1.7kW Spindle, Performance Premium, Recoil, Gantry Lift, Cyclone
Fusion 360
Aspire
Reply With Quote
Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off

Forum Jump


All times are GMT -4. The time now is 05:59 AM.


Powered by vBulletin® Version 3.8.4
Copyright ©2000 - 2021, Jelsoft Enterprises Ltd.