SMH

[BILL HUNTER]

Well, you don't see this very often in expensive cam softwares. Doing a 3d flow on a 3ax VMILL. arcs are filtered in the YZ plane. Post calls up G19. After the process the post does not spit out G17 for the next tool. The next tool is a drill. Drill tries to drill sideways. That usually does not work to well. At least Mastercam has not crashed today...yet.

Don't bother, we already fixed it.

[Rstewart]

The stock standard MPmaster mill post always places a safety line after toolchange

[Smit]

Sounds like a post thing, not a Mastercam thing.

[Guest]

1 hour ago, BILL HUNTER said:

At least Mastercam has not crashed today...yet.

Which version are you using Bill?

[gcode]

These are excellent 3 and 4 axis mill posts .. and they are free

It looks like they have not made the 2021 version available yet

 

MPmaster 3 and 4X mill

https://www.emastercam.com/files/category/32-mpmaster-all-versions/

 

MPLmaster lathe posts

https://www.emastercam.com/files/category/33-mplmaster-all-versions/

 

[nickbe10]

3 hours ago, BILL HUNTER said:

Drill tries to drill sideways.

somebody  has been hacking in YOUR post then.

[BILL HUNTER]

1 hour ago, gcode said:

These are excellent 3 and 4 axis mill posts .. and they are free

It looks like they have not made the 2021 version available yet

 

MPmaster 3 and 4X mill

https://www.emastercam.com/files/category/32-mpmaster-all-versions/

 

MPLmaster lathe posts

https://www.emastercam.com/files/category/33-mplmaster-all-versions/

 

Much thanks. I will try.

1 hour ago, Smit said:

Sounds like a post thing, not a Mastercam thing.

I agree. We changed it to post out : G00 G17 G40 G90 at every tool call now.

[gcode]

5 minutes ago, BILL HUNTER said:

Much thanks. I will try.

Open up the post in a text editor and check out page one..

There are a bunch of switches available to tweak output to your personal needs

[BILL HUNTER]

18 hours ago, nickbe10 said:

somebody  has been hacking in YOUR post then.

We went back and compared the the original post supplied by our vendor. Nowhere was the file altered.

20 hours ago, byte said:

Which version are you using Bill?

2020

[nickbe10]

35 minutes ago, BILL HUNTER said:

We went back and compared the the original post supplied by our vendor.

Quite possibly. These features normally work "out of the box" so somebody has been meddling.

Try running the mplmastter and see, I think you will find these problems will go away, even if your code doesn't look exactly how you want it. Your reseller should be able to fix it for you, especially if you payed for it.

[BILL HUNTER]

Just now, nickbe10 said:

Your reseller should be able to fix it for you

LOL. You have not met our reseller. He is the same guy that told my boss we did not need a verification software for proving NC files because the Mastercam verify was so good.

[nickbe10]

Just now, BILL HUNTER said:

LOL. You have not met our reseller.

No, but I have been in this business using Mastercam to know that all resellers are not created equal. My commiserations.

I am blessed with a responsive and helpful reseller. I have still learned post editing myself, just because it is one of the most powerful tools we have with Mastercam as programmers.

Is your problem post "binned" (encrypted)?

[nickbe10]

50 minutes ago, BILL HUNTER said:

He is the same guy that told my boss we did not need a verification software for proving NC files because the Mastercam verify was so good.

Mastercam Verify is very good for what it is. It is very (very) tool path centric, so it will give you a very good rendition of the cutter motion over say a surface or along a contour. What is does not do (and has never claimed to do), is mimic the "kinematics"  (movements) of the specific machine between cuts. One example of this is dog leg 45 degrees to the long axis in rapid, this could easily cause a crash but is relatively easy to avoid once you understand that MC is of limited help to protect you in ALL circumstances.

Personally I only use CAV for 5 axis work in mills, I don't USUALLY use it on horizontal 4 axis work and never on 4 axis verticals or 3 axis.

I have physically run all these types so much that I am able to visualize the relatively simple motions and clearances in my head (and know when to play it safe).

Lathe I do not have as much experience on and once I get to 2 turrets I am feeling the need for help from CAV. 

Give us an idea of your general type of work you do and I am sure you will get useful suggestions on how to overcome some of the frustrations.

[gcode]

1 hour ago, nickbe10 said:

One example of this is dog leg 45 degrees to the long axis in rapid, this could easily cause a crash but is relatively easy to avoid once you understand that MC is of limited help to protect you in ALL circumstances.

If you properly define your machine's rapid motion on the Linear page of your Control Definition, Mastercam Verify with properly replicate that motion

In the attached example, Verify will dogleg, Check "All axis arrive at destination simultaneously" it will rapid in a straight line.

This has been true since X2 at least

 

[crazy^millman]

1 hour ago, nickbe10 said:

Give us an idea of your general type of work you do and I am sure you will get useful suggestions on how to overcome some of the frustrations.

Tried that and was told to go pound sand so maybe you can make some head way. Good luck!!!

[Colin Gilchrist]

5 minutes ago, gcode said:

If you properly define your machine's rapid motion on the Linear page of your Control Definition, Mastercam Verify with properly replicate that motion

In the attached example, Verify will dogleg, Check "All axis arrive at destination simultaneously" it will rapid in a straight line.

This has been true since X2 at least

 

This feature is in the Control Definition File. It works in conjunction with the "Rapid Feedrate Value", which is defined in the Machine Definition File.

The MD has an option (checkbox) that basically tells Mastercam "All linear axes use the same rapid value", and gives you a parameter box to define that value.

If your machine happens to have different "Max Rapid Rates" for each linear axis, then you'll want to "uncheck" that box. After un-checking that option, you need to go to each of the "Axis Properties" dialog boxes, and in that dialog you can define the "Rapid Rate" for that axis.

Once you've "synced" the settings in the MD and CD, you will see the Dog-Leg moves in both Verify and Backplot (also Machine Sim), since all three utilities are now driven internally by the ModuleWorks engine.

 

[Chally72]

Remember, though, that we don't have knowledge of the acceleration curve of each axis on a machine. Take a Haas VF-2, for example. The X axis sits on the Y axis. The Y, being saddled with more mass to move, is going to be slower to make a rapid move of the same distance than the X. And this all changes again when you load a 400lb casting on the table and try the same thing. This is why seeing dogleg collisions in Verify is nice, but there is still a chance it won't show the exact dogleg collision that WILL happen on your particular machine under your particular circumstances.

It's also why I like to always "Convert rapid to feed" on programs where people insist on using Minimum Vertical Retract on the linking- avoids these situations altogether when I don't have a perfect grasp on machine behavior.

[nickbe10]

39 minutes ago, gcode said:

This has been true since X2 at least

Yes, just using it as an example of "Kinematics".

[BILL HUNTER]

On 9/1/2020 at 8:22 AM, nickbe10 said:

Mastercam Verify is very good for what it is. It is very (very) tool path centric, so it will give you a very good rendition of the cutter motion over say a surface or along a contour. What is does not do (and has never claimed to do), is mimic the "kinematics"  (movements) of the specific machine between cuts. One example of this is dog leg 45 degrees to the long axis in rapid, this could easily cause a crash but is relatively easy to avoid once you understand that MC is of limited help to protect you in ALL circumstances.

Personally I only use CAV for 5 axis work in mills, I don't USUALLY use it on horizontal 4 axis work and never on 4 axis verticals or 3 axis.

I have physically run all these types so much that I am able to visualize the relatively simple motions and clearances in my head (and know when to play it safe).

Lathe I do not have as much experience on and once I get to 2 turrets I am feeling the need for help from CAV. 

Give us an idea of your general type of work you do and I am sure you will get useful suggestions on how to overcome some of the frustrations.

Lately, almost all of my work is 5 axis with quite a bit of multiaxis. What we need is an actual NC file simulator for this. As you said, 5 axis is where you need it. We need it for the same reasons. When there is a mistake in the code that does not show up in mastercam verify we need an alternative. G17/18/19 mistakes (even on 3 axis) could have been caught in a simple g-code verification software (cimco). Just not in Mastercam. In fact, just yesterday the Machine simulator would not simulate a 5-axis drill path because it was drilling from opposite directions on both sides of the part. Does this make sense to you? Not me either. Thanks for the help.

[BILL HUNTER]

On 9/1/2020 at 7:16 AM, nickbe10 said:

Quite possibly. These features normally work "out of the box" so somebody has been meddling.

Try running the mplmastter and see, I think you will find these problems will go away, even if your code doesn't look exactly how you want it. Your reseller should be able to fix it for you, especially if you payed for it.

Yes. My question is, out of what box? Too many times we are given Mastercam post processors that work as if they have never been tested. We were sent a 4 axis vertical Fadal post. No way in heel did anyone ever run 4 axis on that post successfully. I ended up modifying the generic fanuc post to run successfully on the fadal. I really don't have much experience in post writing either. We were sent a 4 axis mori lathe post that would only post out 3 axis code. Perhaps when you say "box" you really mean can. As in garbage can. So, my question is how many more decades will it take before mastercam can ship a quality fanuc or fadal post that actually works? Changing a few M-codes is understandable, but a complete overhaul is inexcusable. Forget trying to get support on posts from our vendor. It won't happen. Whenever I get the support guy on the line the most difficult thing to figure out is whether I am talking to Bevis or Buuthead.

[nickbe10]

1 hour ago, BILL HUNTER said:

Lately, almost all of my work is 5 axis with quite a bit of multiaxis.

I would certainly be looking at a CAV system. 

Vericut is the standard but is not cheap, and takes a fair amount of set up time.

I have heard good things about NCSimul, more reasonably priced, but it is not as well supported.

1 hour ago, BILL HUNTER said:

Yes. My question is, out of what box?

So the first thing I look at is where did the post originate from. Look in the revision log at the top. If you see the initials IHS then it is originally an In House Solutions post. If you see CNC then it came from Mastercam originally. Most are edited versions of there generic posts.

This can help you track down the "source post". Now you can run a file compare with your problem post to start figuring out the problems. Do you have the documentation? Have you used the debugger? 

1 hour ago, BILL HUNTER said:

So, my question is how many more decades will it take before mastercam can ship a quality fanuc or fadal post that actually works?

Just remember unless you get a post from the tech exchange at CNC (have you looked there?) you are not necessarily getting a post from Mastercam, you are getting a post from a reseller and so may be limited by their skills and knowledge.

Dialing in posts isn't easy at the best of times, and over the phone or indirectly inevitably leads to a tail chase or back and forth a few to many times. That's why I (and I suspect others) took matters into our own hands and do it ourselves. All my posts are MPMASTER derived and I am able to constantly control the updates and improvements, and keep them consistent. And 90% of the modifications are very straight forward, but make a significant difference at the machine.

[Greg Williams]

I have found MPmaster and MPLmaster to be a good starting point

[Guest]

 

On 9/1/2020 at 7:35 AM, BILL HUNTER said:

We went back and compared the the original post supplied by our vendor. Nowhere was the file altered.

I'd shoot your reseller an email with an attached zip2go file. Mastercams official forum has a post section where cnc software has experts in the field who can offer some help.

If this is an issue with mastercam, please contact [email protected]

[BILL HUNTER]

On 9/5/2020 at 12:17 AM, byte me said:

 

I'd shoot your reseller an email with an attached zip2go file. Mastercams official forum has a post section where cnc software has experts in the field who can offer some help.

If this is an issue with mastercam, please contact [email protected]

That is a great recommendation. However, we did shoot a zip2go to mastercam qc support. Never got help.

[Guest]

1 minute ago, BILL HUNTER said:

That is a great recommendation. However, we did shoot a zip2go to mastercam qc support. Never got help.

It's possible they missed your email, I imagine their inbox must be overflowing at sometimes, I would send a follow up email, and if still nothing maybe give them a phone call, a post on the official forum sometimes can get traction to, particularly with the PROBLEM tag selected.