Recommended Posts

 

48 minutes ago, motor-vater said:

What am I doing wrong?

I don't think you are doing anything wrong....

This looks like a Post Processor issue, someone has fat fingered an extra R in a format or postline statement

Share this post


Link to post
Share on other sites

You can use the debugger and find that exact line.

Share this post


Link to post
Share on other sites

NEVER USED THE DEBUGGER????? I wouldnt know where to start... lol

seems like this might be the area maybe the mr2$ is allready adding the "R"??

MR2.PNG.6d1fcf013c9dffc68327d674317e69e5.PNG

Share this post


Link to post
Share on other sites

Backup your file, with a different name.

Change this:

      if mr1$ = 2, #AI-NANO 2, AI(nano)CC output (Artificial Intelligence Contour Control) - G05.1 Q1
        [
        pbld, n$, *sg49, e$                                            #Must be in G49 and remain before G43
        if ipr_type > 1, ipr_type = 0                                  #Must be in G94
        pbld, n$, sgfeed, e$
        pbld, n$, "G05.1", "Q1", [if mr2$, "R", no_spc$, *mr2$], e$    #Mr2 gives accel/decel value/coefficient, usually R or P
        mr1_flg = 2
        ]

To this:

      if mr1$ = 2, #AI-NANO 2, AI(nano)CC output (Artificial Intelligence Contour Control) - G05.1 Q1
        [
        pbld, n$, *sg49, e$                                            #Must be in G49 and remain before G43
        if ipr_type > 1, ipr_type = 0                                  #Must be in G94
        pbld, n$, sgfeed, e$
     #   pbld, n$, "G05.1", "Q1", [if mr2$, "R", no_spc$, *mr2$], e$    #Mr2 gives accel/decel value/coefficient, usually R or P
        pbld, n$, "G05.1", "Q1", *mr2$, e$ #Mr2 gives accel/decel value/coefficient, usually R or P
        mr1_flg = 2
        ]
  • Like 1

Share this post


Link to post
Share on other sites

That change is just for the phsm1_on section

I don't know if it would be needed in your phsm2_on section or not.

Share this post


Link to post
Share on other sites

man thanks again for this Guru, I'm like a kid at Christmas with this right now. This Mori Hori I programmed was shaking and making a mess of some surfaces I was trying to machine, and even worse running slower than a 1 legged dog on 4 axis moves.... Some look ahead and now its smooth and fast... I even shaved a few minutes off some optirough paths with it today... Super happy, now if I could just get it to spit out a G332 and the G05.1, I would be able to do it all with out editing any code, that would be real nice

  • Like 1

Share this post


Link to post
Share on other sites

You could try replacing this:

      if mr1$ = 2, #AI-NANO 2, AI(nano)CC output (Artificial Intelligence Contour Control) - G05.1 Q1
        [
        pbld, n$, *sg49, e$                                            #Must be in G49 and remain before G43
        if ipr_type > 1, ipr_type = 0                                  #Must be in G94
        pbld, n$, sgfeed, e$
     #   pbld, n$, "G05.1", "Q1", [if mr2$, "R", no_spc$, *mr2$], e$    #Mr2 gives accel/decel value/coefficient, usually R or P
        pbld, n$, "G05.1", "Q1", *mr2$, e$ #Mr2 gives accel/decel value/coefficient, usually R or P
        mr1_flg = 2
        ]

With this:

      if mr1$ = 2, #AI-NANO 2, AI(nano)CC output (Artificial Intelligence Contour Control) - G05.1 Q1
        [
        pbld, n$, *sg49, e$                                            #Must be in G49 and remain before G43
        if ipr_type > 1, ipr_type = 0                                  #Must be in G94
        pbld, n$, sgfeed, e$
     #   pbld, n$, "G05.1", "Q1", [if mr2$, "R", no_spc$, *mr2$], e$    #Mr2 gives accel/decel value/coefficient, usually R or P
     #   pbld, n$, "G05.1", "Q1", *mr2$, e$ #Mr2 gives accel/decel value/coefficient, usually R or P
        pbld, n$, "G332", *mr2$, e$ #Mr2 gives accel/decel value/coefficient, usually R or P
        pbld, n$, "G05.1", "Q1", e$
        mr1_flg = 2
        ]

The G332 line may need the "R", which would mean that line would be:

                 pbld, n$, "G332",   [if mr2$, "R", no_spc$, *mr2$], e$ #Mr2 gives accel/decel value/coefficient, usually R or P

Again, I can't stress enough, make a backup before making changes to you post.

 

Share this post


Link to post
Share on other sites

Could somebody explain me the "artificial intelligence" part of AI Nano contour control option?

Share this post


Link to post
Share on other sites

Wow just learned an expensive lesson about stringing 2 toolpaths together with G05.1 and Not using a forced tool change.... G49 is bad.... with out a new G43

Share this post


Link to post
Share on other sites
3 hours ago, SlaveCam said:

Could somebody explain me the "artificial intelligence" part of AI Nano contour control option?

Fanuc will tell you AI doesn't stand for that. But I'm sure all those years ago when they released it (mid 90's?) that's what they were calling it.

Anyway, it's another set of parameters used for acc/dec and the algorithm looks ahead and processes the path so the machine "knows where it's going to go".

Share this post


Link to post
Share on other sites
4 hours ago, motor-vater said:

Wow just learned an expensive lesson about stringing 2 toolpaths together with G05.1 and Not using a forced tool change.... G49 is bad.... with out a new G43

What Post are you using Pete?

The MPMaster Post has logic for detecting if any values between Operations has changed, and the Post will retract Z home, cancel TLO (G49), then output the new XY position, and approach with a G43 Z move to enable TLO again.

There is a lot of logic that is needed to track which mode is active. Plus, there is logic to detect a different 'R' value, which means the Post will cancel the active G05.1 mode, then it will output G05.1 again with the new R value.

I'd highly recommend updating your Post to use the latest High-speed logic from MPMaster.

Share this post


Link to post
Share on other sites

its definitely an older MP Master, that has been through the migration a lot of times.... Something else for the Colin list... lol

Share this post


Link to post
Share on other sites
5 hours ago, motor-vater said:

Wow just learned an expensive lesson about stringing 2 toolpaths together with G05.1 and Not using a forced tool change.... G49 is bad.... with out a new G43

I just ran into this bug the other day.  Can't start up G5.1 at a null Tool change.  By default this happens if you use a drill cycle followed by anything else with the same tool....   I didn't learn the hard way so to speak, but did scrap a really cheap part.

It's and easy fix, and I did it, but it made up mind the other day that I am going to be moving away from the MPMASTER.  I keep running into issues, and it is a difficult post to make edits to given its shortcomings from a structure perspective.  I know it's been the gold standard for many years, but after reading through one of the recent releases of the MPFAN post from CNC I will be adding my needed functionality to it as it is a far easier post to follow and make "simple" edits to.

I know they are based on the same post but it seems the recent maintenance to the MPFAN post has been very good, clean, effective and mostly up to date with current practices.  I just feel the MPMASTER needs a serious revamping to condense functions and whatnot.

The G49 issue with G5.1 wouldn't be an issue if there were a few safeties put in place to keep track of length comp, something I have done for years in my 5axis posts as wcs changes require dropping G43.4.  Once you start keeping track of that status you can put error handling to make sure comp is on at the end of you toolchange and null toolchange sections.  But moreover you should only really have two places in your post here length comp is turned on and you can only turn it off in a routine that will eventually lead to it getting turned back on.

 

Share this post


Link to post
Share on other sites

I took a quick look at the mpmaster after Pete posted about his crash. I didn't see the logic to reset G43.4 on a null tool change, but I didn't have time today for a thorough look-see.

I'm gonna take a better look this weekend, if I get a chance.

Share this post


Link to post
Share on other sites

I just need a G43 H#, Yeah $200 doller endmill into a $500 piece of material... Took that good feeling away real quick.. Vericut was no help cause I need to modify the G49 area in there it always alarms out at a G49... Lesson learned always check your code when trying new stuff

Share this post


Link to post
Share on other sites

I always turn off motion on G49.  I've had that burn me.

Share this post


Link to post
Share on other sites
9 hours ago, jlw™ said:

I always turn off motion on G49.  I've had that burn me.

That's one of the first things I check on a new machine.  Also, default to G49 when reset is pressed.  That one will make you scratch you head for a minute until you realize that's why the machine keeps alarming out.  Stock MPMASTER i was last playing with didn't have a G49 in the header.  FWIW, all modal codes possibly used should be in your header of any posted code.....

Share this post


Link to post
Share on other sites

I wish the Generic Fanuc 4X Mill Post had the same High Speed Code logic that MPMaster has. I love the default Posts from CNC Software, but they are just missing some "standard" features that are commonly available these days.

Both MPMaster and the Generic Fanuc 4X Mill Post have logic that defaults to G91 G28 for retracts.

I despise G28 home position moves, because some machines will "reference return", which means they "go to Zero first, before going Home".

I like to modify all my Z retracts to use the following:

G00 G90 G53 G49 Z0.

The reason is because the G53 code is always Non-Modal. Meaning it is only active on the line it is called on, and it won't cancel your active Work Offset. It also never "goes to WO zero, before going home".

You can opt not to include the G49, if you are keeping G43 active, but if you want to "cancel TLO", while also going to "Z Home", that is the safest way to do it.

And yes Pete, getting Vericut properly configured to detect crash behavior is a must!

 

Share this post


Link to post
Share on other sites
7 hours ago, Colin Gilchrist said:

And yes Pete, getting Vericut properly configured to detect crash behavior is a must!

This is kinda the whole point. 🧐

  • Like 1
  • Haha 1

Share this post


Link to post
Share on other sites
22 hours ago, jlw™ said:

I always turn off motion on G49.  I've had that burn me.

That is if the parameter for movement when called is on or off. Amazing how many of the builders still use the default parameter of movement when G49 is called. Just had 6 different brand new machines need to have this turned off in the last year. 

People le from what I have seen as of late never properly vet their Vericut. Even the best vetting so to speak there is still the .01% Vericut will miss. I have debugged about 20 different machines in the last few years that were quote unquote proven Vericut machines. I don’t put the blame on CG Tech or any CAV company. Problem is most companies never want to do it right. They want it good enough and call it a day. 

  • Like 2

Share this post


Link to post
Share on other sites

got VERICUT dialed in today, that helps major. I love that stuff... Found a few more problems in there that I am glad I never came a cross on the control. The null tool change is the least of my problems. lol turns out that if you are trying to use multi passes on something like a 5 axis curve (in 4 axis for my case) every time it picks up to come back for the finish pass, bam! another G49, G05.1, with out a G43..... I am in the danger zone with this stuff for sure. But man it works so good on the machine.

I spent about an hour reading through the mori book and it gives u tidbits of useful info like I am calling a R# after my "G05.1 Q1 R#".. But it appears, at least according the book the R# does nothing. Q1=on, Q0=off that simple. But something the book mentions that instantly made me pucker was that any rapid move temporally cancels the look ahead and then turns it back on after the rapid. YIKES! I usually program my retracts as feed moves in opti-programs but I am hoping that this does not have adverse affects on toolpaths with rapid moves???

I'm gonna download the newest MPMaster and just see how it posts out.. I'm pretty sure it works right out of the box for the Mori code, select horizonal and not haas in the switches and I think its gonna give me the same code, but hopefully with more logic.

Share this post


Link to post
Share on other sites

Happy to report the new MP Master looks like a winner in this... Thanks Colin! Right out of the box it seems to do everything I need, just leaves the G05 on through null tool changes, turns it off when its supposed to, and doesn't seem to ever post it without a g43....

The only bad thing about this was it just cost the company$$$ for me to update to newer post, thankfully this was a set up piece but still I would have liked to first article it for data.... Better be real good on the next one! when I have time I'll fish around for info on how to change one of the misc reals into a switch for G332, I'm sure its been discussed on here. Thanks again everyone!

  • Like 1

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us