Hello Guest it is October 22, 2019, 08:11:59 AM

Author Topic: Problem with MACH3 and first peck drill cycle  (Read 8896 times)

0 Members and 1 Guest are viewing this topic.

Re: Problem with MACH3 and first peck drill cycle
« Reply #10 on: September 25, 2016, 03:38:37 PM »
OK, hopefully a LAST post from me regarding this issue.

I just installed the older version of Mach3, version 062 to see how it handles the G64 code and it behaves the same as version 066. So, I'll just make sure I don't use G64 in the header of any of my jobs.

Not sure if I'll go back to version 066 or stay at 062 since both appear to have the same issues.

I should probably think about moving to Mach4 but will have to rewrite a dozen scripts or more when I make the move. I'm a bit confused on the Mach4 licensing, I'm a hobbyist and I currently use the same licensed copy of Mach3 on my CNC Mill and CNC Router, two separate PCs. Will I have to purchase two Mach4 hobby licenses if I switch or can I just generate two keys, one for each PC via the single Mach4 hobby license?

Thx,
Joe
Re: Problem with MACH3 and first peck drill cycle
« Reply #11 on: September 25, 2016, 06:33:47 PM »
So much for a last post.....

I'm now getting the bad peck cycle even with the G64 code removed. I SWEAR I was able to verify earlier the G64 code was causing the problem but now it doesn't appear to be. One thing for certain (I think) is that if I let the first peck drill operation complete, albeit screwed up, then all following peck drill cycles work properly. Even if I load a new job, they all continue to work properly. If I then terminate Mach3 and restart it, I get the problem again, until I let it complete one screwed up peck drill cycle. I've also seen the first peck drill cycle work properly if I run some other job first, even if the job does not have a drill cycle in it. I'm a retired software engineer and it just appears to me that some internal Mach3 variables key to the peck drill cycle are not getting initialized properly when Mach3 first starts up.

I'm really tired screwing with this but I need a reliable peck drill function. I'm really surprised others have not run into this, perhaps most others are using the old printer interfaces and they don't seem to have this problem, only smart controllers.

Offline rcaffin

*
  •  1,003 1,003
    • View Profile
Re: Problem with MACH3 and first peck drill cycle
« Reply #12 on: September 25, 2016, 06:51:34 PM »
it just appears to me that some internal Mach3 variables key to the peck drill cycle are not getting initialized properly when Mach3 first starts up.
This is far more likely. We already know that it can take two spin commands (eg S100) to get the spindle spinning at the required speed at the start.

As a ridiculous and horrible (but probably quite effective) work-around, you could consider inserting a dummy G83 command at the start - up in the air without any drill bit for instance. How about trying the idea out and reporting back?

Cheers
Roger
Re: Problem with MACH3 and first peck drill cycle
« Reply #13 on: September 27, 2016, 03:56:14 PM »
Well, I think I have a way to make the peck drill cycle work properly on the first and all proceeding drill cycles.

The problem I’ve been fighting is definitely related to the machines “Velocity Mode” when the job starts. If the mode is set to “Constant Velocity”, G64, the first peck drill cycle will not work properly and will jam the drill bit down to the final hole depth on each peck retract cycle. After the first hole, all following peck drill operations will work properly.

I’ve found that if I explicitly put Mach into “Exact Stop” velocity mode, either by including the G61 code in Mach’s initialize string or by including G61 in the jobs G Code file header, all the peck drill cycles work properly, including the first. If I omit the G61 from the initialize string AND the job G Code header, the first peck drill cycle fails.

So, to be safe (hopefully), I have included G61 in Mach’s initialize string AND will include it in the header of all my CamBam generated G Code files.

Thanks for all the input and suggestions:

Offline rcaffin

*
  •  1,003 1,003
    • View Profile
Re: Problem with MACH3 and first peck drill cycle
« Reply #14 on: September 27, 2016, 05:05:10 PM »
Interesting.

Now, I wonder ... what happens if you put G61 into the Mach initialise string, and G64 into the CamBam header?

Cheers
Roger
Re: Problem with MACH3 and first peck drill cycle
« Reply #15 on: September 27, 2016, 05:06:43 PM »
It fails.

Offline rcaffin

*
  •  1,003 1,003
    • View Profile
Re: Problem with MACH3 and first peck drill cycle
« Reply #16 on: September 27, 2016, 05:13:45 PM »
How very odd.
But not entirely unexpected. It would seem that it is not just in starting Mach3 that there are some 'funnies', but also in loading a program. Sigh.
Cheers
Roger
Re: Problem with MACH3 and first peck drill cycle
« Reply #17 on: March 28, 2018, 08:38:50 AM »
 I am having a similar problem with a G81 cycle. I can run the program once ,and then it will not react to the Feed code and just  rapid into the work. If I restart Mach 3 it is fine again for the first run. I am going to check tonight using G61 inserted.

Rick.

Offline rcaffin

*
  •  1,003 1,003
    • View Profile
Re: Problem with MACH3 and first peck drill cycle
« Reply #18 on: March 31, 2018, 03:13:39 AM »
Right now I cannot see why G81 would be affected by G61. It is not possible to run a drill cycle in anything other than 'exact stop'.
I have not had any problems with repeated G8x cycles.

Cheers
Roger
Re: Problem with MACH3 and first peck drill cycle
« Reply #19 on: March 31, 2018, 06:52:31 PM »
 Here is what my machine is doing. Let's say we are drilling 4 holes , .75 spacing on the x axis , G81 cycle f10.0. I am using MACH3  ver 062 with ess, windows xp.
My machine rapids at 100 ipm , and usually I have the rapids turned down until I know things are going right. If I set the rapids to 50% as Mach boots up ,the first run is
fine, but by the 2nd or 3rd  run it will just always move at the reduced rapid feed rate all the time , and if I take off the rapid overide while still in run mode , then it just moves at 100% rapid. Does not matter if g64 ,or g61 is model , I tried it both ways.
 I did notice when it does this , the feed rate displays the rapid feed of 50 ipm , when usually this would always display the commanded F10.0 , unless the feed rate changed in the program. I have to reboot Mach in order to clear this.
 Now if I have rapids set 100% when I first boot it up , and run the program at least once , it seems ok and I can even lower the rapids after that.
 Anybody ever experience this?

Rick.