Topics Topics Edit Profile Profile Help/Instructions Help    
Search Last 1|3|7 Days Search Search Tree View Tree View  

Tool change pauses

IMService Discussion Forum » DeskCNC support discussions » Tool change pauses « Previous Next »

Author Message
Top of pagePrevious messageNext messageBottom of page Link to this message

David Waine (Aussiedude)
New member
Username: Aussiedude

Post Number: 1
Registered: 08-2003
Posted on Thursday, August 28, 2003 - 01:27 am:   Edit Post Delete Post View Post/Check IP Print Post    Move Post (Moderator/Admin Only) Ban Poster IP (Moderator/Admin only)

Hi, I would like to know if ther is a way to have my machine do a minium of a pause or even better go to a "tool change" posityion between engraving and each different drill bit size when building PCBs.
Any suggestions other than manually adding g-code into the nc file?
Is ther a setting somewhere or would some kind of mod to the post processor do it?

Sincerely

David
Top of pagePrevious messageNext messageBottom of page Link to this message

support (Support)
Moderator
Username: Support

Post Number: 804
Registered: 01-2002
Posted on Thursday, August 28, 2003 - 09:11 am:   Edit Post Delete Post View Post/Check IP Print Post    Move Post (Moderator/Admin Only) Ban Poster IP (Moderator/Admin only)

DeskCNC defaults to placement of an M06 to effect a tool change. This command should cause any machine without a toolchanger to pause until the user presses the "start" button.

Sample code:

(Created 9:12:38 AM 8/28/03 from Advanced.dxf)
(Post = ISO G-Code - Non Modal)
(Tool 7 = 20 Degree Conical)
N0001 T7 M06 S10000

Are you saying that your machine does not do this, or that you don't think that DeskCNC is creating this kind of code?

You can control the tool change activity using a tool change "macro". Check the DeskCNC help file under "Other files used by DeskCNC", for information about using this capability.

Fred Smith - IMService
Top of pagePrevious messageNext messageBottom of page Link to this message

support (Support)
Moderator
Username: Support

Post Number: 811
Registered: 01-2002
Posted on Wednesday, September 03, 2003 - 09:57 am:   Edit Post Delete Post View Post/Check IP Print Post    Move Post (Moderator/Admin Only) Ban Poster IP (Moderator/Admin only)

In trouble shooting with another customer, I have discovered that some builds of DeskCNC may have been distributed, without a pause built into the tool change code. This pause is found as an M0 in the toolchange.cfg file.

At a minimum, this file must contain the following lines:

[TOOL1]
PICKUP0=M0 (*** program stop until tool has been changed)


It is not necessary to add additional tools, as Tool1 is assumed unless other tools are added. See the help file under "Other Files used by DeskCNC" for more info about the Toolchange macros.

Fred Smith - IMService
Top of pagePrevious messageNext messageBottom of page Link to this message

David Waine (Aussiedude)
New member
Username: Aussiedude

Post Number: 2
Registered: 08-2003
Posted on Monday, October 06, 2003 - 10:55 am:   Edit Post Delete Post View Post/Check IP Print Post    Move Post (Moderator/Admin Only) Ban Poster IP (Moderator/Admin only)

OK, so rather than just pause I would like my machine to: 1) lift up to a specified Z height, 2) turn off the spindle and then 3) go to a specified XY coordinate.
After I have manually changed the tool and hit the pause button or some such it should turn back on the spindle and continue on.
Could someone (Fred?)post the appropriate cfg file on here so others could refer back to it also.
Thanks in advance

David
Top of pagePrevious messageNext messageBottom of page Link to this message

support (Support)
Moderator
Username: Support

Post Number: 861
Registered: 01-2002
Posted on Monday, October 06, 2003 - 02:28 pm:   Edit Post Delete Post View Post/Check IP Print Post    Move Post (Moderator/Admin Only) Ban Poster IP (Moderator/Admin only)

David,

Write the G-code that you want to occur at a tool change callout and post it here. Then we can show you how easy it is to format your tool change callout.

Fred Smith - IMService
Top of pagePrevious messageNext messageBottom of page Link to this message

support (Support)
Moderator
Username: Support

Post Number: 868
Registered: 01-2002
Posted on Monday, October 13, 2003 - 12:40 pm:   Edit Post Delete Post View Post/Check IP Print Post    Move Post (Moderator/Admin Only) Ban Poster IP (Moderator/Admin only)

Here is some sample code to try

(This is a comment it is ignored by the G-code parser)
G00 Z1.0 (raise tool to Z =1.0)
G00 X1.0 Y1.0 (rapid to position X=1.0 Y=1.0)
M05 (spindle off)
M09 (Coolant off)
M00 (Program stop, waits while you change your tool, press go to continue)
S15000 M03 (Spindle on clockwise 15,000 RPM)
M07 (Coolant on)

Place the above lines in the Toolchange macro file preceeded by control lines arranged like this:

[TOOL1]
PICKUP0=G00 Z1.0 (raise tool to Z =1.0)
PICKUP1=G00 X1.0 Y 1.0 (rapid to position X=1.0 Y=1.0)

etc.

You should be able to place the G-code listed above in a text file and run it to test that it executes the desired sequence of steps. Then place it in the tool change macro AFTER you test it. Let us know how it works.

Fred Smith - IMService

Administration Administration Log Out Log Out   Previous Page Previous Page Next Page Next Page