Calypso CNC User Forums

CVI Announcements

IMPORTANT NOTICE - Mach3 vs Win10 1803 - read this post!

http://www.calypsoventures.com/forums/viewtopic.php?f=4&t=519

MSM 2.3.14 is the latest release.

Due to Spamming, we've had to make all posts from new members require approval before they show up.
After the first few posts are approved, your posts will show up normally. Sorry for the extra latency.


M998

MSM Mill mode support

M998

Postby tmostad » Sun Apr 06, 2014 8:19 pm

I am trying to implement the probe as master tool setup strategy and am having problems. I have a PCNC1100 so I started with the Tormach supplied XML file for it when initially configuring MSM. The problem I am having is that on a tool change the Z axis hits its "+ limit" which then of course dereferences the machine and causes all kinds of problems for me. I am using SprutCAM with the Tormach post processor which generates an M998 which I believe is Tormach's tool change macro and I think the root of the problem. The question I have is: Is M998 used by MSM for anything? I searched the User's Manual and the forum for "M998" and found nothing so I assume it will be safe to remove it from the post processor...?
tmostad
 
Posts: 14
Joined: Tue Oct 29, 2013 1:14 pm

Re: M998

Postby DaveCVI » Mon Apr 07, 2014 10:24 am

Hi,
tmostad wrote:I am trying to implement the probe as master tool setup strategy and am having problems. I have a PCNC1100 so I started with the Tormach supplied XML file for it when initially configuring MSM. The problem I am having is that on a tool change the Z axis hits its "+ limit" which then of course dereferences the machine and causes all kinds of problems for me.

The tool change position for MSM is set on the tooling page. Note the position is stored and accessed in machine coordinates. If going to the TCP is causing the machine to hit the Z+ limit switch, then move the TCP down a bit in Z so that the switch is not triggered.

Most machine set machine coord Z = 0 to be the top of travel in Z. This is usually where the home switch is triggered. It's also unusual (but not impossible) to not be able to go to the Z home position w.o triggering the Z limit. Generaly, moving Past the Z home position should trigger the limit, but not moving to the home position.

tmostad wrote:I am using SprutCAM with the Tormach post processor which generates an M998 which I believe is Tormach's tool change macro and I think the root of the problem. The question I have is: Is M998 used by MSM for anything? I searched the User's Manual and the forum for "M998" and found nothing so I assume it will be safe to remove it from the post processor...?

M998 is a Tormach specific script. The comment at the start of the M998 script says:
"' This macro implements Goto Tool Change logic "
Since you re using the tool change position in MSM, there is no need for the tormach M998 macro.
There are two ways to "disable M998"
1) remove it from the Sprutcam post processor output so there will not be a call to M998 in the generated code. The details of how you do that I am not familiar with as I do not run Sprutcam.
2) replace M998 in your macro directory with an empty script. Then even when the M998 script is called, it won't do anything.

Dave
Productivity Software for Personal CNC Machinists
http://www.CalypsoVentures.com
User avatar
DaveCVI
Site Admin
 
Posts: 754
Joined: Mon Feb 04, 2013 2:15 pm

Re: M998

Postby tmostad » Mon Apr 07, 2014 3:21 pm

Thanks Dave. I found in the post processor where the M998 was generated and commented it out. It now doesn't appear in the G code but unfortunately it doesn't solve the problem. I have narrowed it down to this line:

T2 G43 H2 M6

If I manually enter T2 M6 then there is no problem. If I enter the whole line it causes the Z axis to hit the + limit switch. Is the G43 H2 necessary for MSM tool change or any other MSM function?

Thanks,

Tim.
tmostad
 
Posts: 14
Joined: Tue Oct 29, 2013 1:14 pm

Re: M998

Postby DaveCVI » Mon Apr 07, 2014 3:58 pm

Ah... That is a known bug in mach 3. See MSM release notes item 4.27 for more into.
Alas, it's just one of many bugs reported to Artsoft that have not been (and apparently will not be) fixed.

Change the post to do two lines:
T# M6
G43 H#

Dave
Productivity Software for Personal CNC Machinists
http://www.CalypsoVentures.com
User avatar
DaveCVI
Site Admin
 
Posts: 754
Joined: Mon Feb 04, 2013 2:15 pm

Re: M998

Postby tmostad » Mon Apr 07, 2014 5:43 pm

Yep that was it! Oddly enough the preprocessor comes right from Tormach and it outputs this code. You'd think that they would know better. I'll be sure to tell them.

I also solved a different problem that has been nagging me by changing out a parallel port cable. Two big breakthroughs in one day. I might as well buy a lottery ticket and make it three!

I believe that this will solve my G55 probing problem also (as documented in another forum post). I'll be sure to follow-up on that one too.

Thanks for your help!

Tim.
tmostad
 
Posts: 14
Joined: Tue Oct 29, 2013 1:14 pm

Re: M998

Postby DaveCVI » Mon Apr 07, 2014 9:53 pm

Great!

tmostad wrote:Yep that was it! Oddly enough the preprocessor comes right from Tormach and it outputs this code. You'd think that they would know better. I'll be sure to tell them.

I believe the bug is only in mach 3.43.xx, Since Tormach ships only a old 2.xx.xx with the Tormach machines, they probably don't encounter this bug. This is an example of why Tormach ships a very old version of mach and only supports it - they know what bugs are in that old version.

Dave
Productivity Software for Personal CNC Machinists
http://www.CalypsoVentures.com
User avatar
DaveCVI
Site Admin
 
Posts: 754
Joined: Mon Feb 04, 2013 2:15 pm


Return to MSM Mill Support

  • Who is online

    Users browsing this forum: Bing [Bot], Google [Bot] and 59 guests

cron