How to address Dog Leg Rapids in the X7 Verify- or "why does verify show gouges that aren't there?"

[Guest]

 

 

Freedom of speech.....

If you can do it so can he.

 

Actually yelling "FIRE" in a crowded movie theater is NOT freedom of speech and can be prosecuted for any number of crimes from aggravated mayhem to inciting a riot.

[Thee Rickster ™]

James, you are right, i was wrong, thinking it had anything to do with freedom of speech.

 

I would have thought the same thing as the original post, until gcode

expertly pointed out the non concern and solution.

 

i meant freedom to voice concerns....... they both won.

[Bridgeportboy]

I came to be a Mastercam user a couple of years ago when the company I work for

acquired the assets of another company that was going out of business.

Included in that purchase was a Parpas Master P 5 Axis milling machine, a seat

of Mastercam X4, and the post for that machine.

 

It was my responsibility to learn Mastercam and how to run this, our first 5 axis machine,

at the same time. All I had to go on was the fact that this machine was programmed with

Mastercam before and that the post was proven and working correctly.

 

I can honestly say that my butt was in a constant state of pucker and my heart in my throat

every time I went to depress the cycle start button those first few months.

If something didn’t look right, I had to figure out if it was me, Mastercam, or the machine that was causing the issue.

Thankfully, it was ME messing up almost every time and a chance to learn something.

 

My reseller worked tirelessly with me on phone support, working through issues at hand, and I wouldn’t

be where I am today without their help. This forum has also been a treasure trove of valuable information

and I am glad to be a part of it. Thank you to all who take the time to respond with tips or pointers for us

members that are still trying to improve our MC and machining skills.

[Newbeeee™]

^^^well said. This forum has such a w I d e spread of knowledge - not just mcam but mtls. tooling, machines, methodology etc.

And no-one hesitates to share that knowledge. It is pretty exceptional to be honest.

And there's a fair good bit of p1ss taking as well which helps

[Tyler Robertson]

a suggestion: how about pinning a topic about verify and dog leg moves

 

i realize it's in the what's new section but as gcode pointed out we are all guilty of not reading it or skimming it at best. jmho

 

I agree, how about I pin this one? Does a good job of explaining the issue someone sees, and how the feature is to be used?

[crazy^millman]

Might change the topic from "False" to "How to address Dog Leg Rapids in the New Verify".

[Tyler Robertson]

Might change the topic from "False" to "How to address Dog Leg Rapids in the New Verify".

 

yep

[bogusmill]

Does the setting shown affect only verify/backplot or does it change the output of the .nc code?

 

I am working with our reseller to get a decent working post for our Haas VR-8. It's a head-head 5 ax machine. I was testing the post using a program with peck drilling on a vector but staying above the actual part. In a 3 axis machine your peck is a rapid out and back in then drill at feedrate. But I noticed on vector holes that there was dog legging on the retract and return to next peck which would be devastating if actually cutting metal. The post developer set up the machine and control defs he wanted me to use so I didn't even notice these settings.

[gcode]

In my experience, the setting on the rapid page only effect what happens in the UBVS.

You need to get your post developer to change the post to G01 rapid during 5 axis drilling

or

review your Haas parameters manual.

There may be a setting that forces the machine to straight line rapid

[Müřlıń®]

I don't know why posts don't default linear moves for rapids in the first place.

Aren't G0's mainly used to cancel canned cycles, cancel model codes and cutter comp and Crash Machines?

 

BTW This is a good thread....need to know information here....

[gcode]

I don't know why posts don't default linear moves for rapids in the first place.

Aren't G0's mainly used to cancel canned cycles, cancel model codes and cutter comp and Crash Machines?

 

BTW This is a good thread....need to know information here....

 

There is a switch in the Control Definition to force G01 rapid motion if that's something you would like to do

[Müřlıń®]

There is a switch in the Control Definition to force G01 rapid motion if that's something you would like to do

 

Ya I know there's one now...I was just saying I think the default setting should have always been set to use G01"s (starting back in 1982 until now).....and everyone who needs G0's turn on the switch .....

 

Many users with less experience would have a much better Mastercam experience If it were.

[Aaron Eberhard]

I don't know why posts don't default linear moves for rapids in the first place.

Aren't G0's mainly used to cancel canned cycles, cancel model codes and cutter comp and Crash Machines?

 

BTW This is a good thread....need to know information here....

 

It's a good question in for modern machines, but coming from the control side, I do know that on old machines, it used to be a completely different feed algorithm than G01s.. The old machines/controls used to have "controlled (G01)" vs "uncontrolled (G00)" speed readings.

 

Perhaps it has to do with the fact that all of the machines that could use a lot of posts have different max rates, and some controls will error out if you give it too high of a feedrate (instead of just interpreting it as "as fast as possible")?

[Newbeeee™]

Aaron - I'm sure all machines still run the same way - as in a different set of algorithm's for G00 and G1.

Funac's have different parameters for acc and dec etc for the two states as well as bell shape or linear choices..

[Ben Wood]

I don't know why posts don't default linear moves for rapids in the first place.

Aren't G0's mainly used to cancel canned cycles, cancel model codes and cutter comp and Crash Machines?

 

BTW This is a good thread....need to know information here....

 

Using G00 I can have separate overrides for rapid and feed. I always run the first part at 25% rapid override but leave my feed at 100%.

[mdlmkr]

In earlier versions of Mastercam Verify and Backplot rapided in straight lines.

This was fine if your machine ran in straight lines, but many dogleg and this forum is full

of threads where people complained that Verify was good, but the part got hit anyway.

That's because their machine ran dogleg rapid motion and Verify couldn't simulate it.

New for X7, Verify can run straight or dogleg, depending on how you've set the Rapid Motion

setting in your Control Definition.

See the attached screen shot..

This is how you'd set it for a machine that doglegs.

 

My settings already agreed with these, and I still have the issue, verify is showing gouge and it also shows when I look at the backplot, it definitely has to do with retract, but how can this be addressed? This is a major problem for me an our team.

 

Try changing it to " All axes arrive at destination simultaneously"

 

That's how a machine that runs in a straight line should be set

[DavidB]

I have question.

If Mastercam can do doglegs in verify and show gouges that will occur. Why doesn't Mastercam using the machine setup info avoid these gouge's?

 

In a HS Toolpath you can set a minim retract to miss the work piece. But Mastercam will gouge here if your machine dog legs. So the answer is to do a full retract. This adds cycle time to your jobs.

 

Cheers Dave

[gcode]

I have question.

If Mastercam can do doglegs in verify and show gouges that will occur. Why doesn't Mastercam using the machine setup info avoid these gouge's?

 

In a HS Toolpath you can set a minim retract to miss the work piece. But Mastercam will gouge here if your machine dog legs. So the answer is to do a full retract. This adds cycle time to your jobs.

 

Cheers Dave

 

in 3D high speed footpaths you can define your retracts as G01 rapids and dog legs are not an issue

[DavidB]

Good point Gcode

 

But I was just wondering if MC knows it will hit the part with this dogleg motion why cant it adjust the retract height so it misses the part?

[gcode]

Good point Gcode

 

But I was just wondering if MC knows it will hit the part with this dogleg motion why cant it adjust the retract height so it misses the part?

UBVS does not know if rapid motion will hit a part or not, it is just accurately emulating that motion.

The 3D high speed tool paths do have stock awareness and can avoid it. Hopefully this awareness will migrate to other toolpaths

in future releases.

Hint.. for a good laugh, set a 3D high speed toolpath to minimum clearance (.250" clearance and G01 = 500)

Then stand back and watch your operators face as he proves the program out

[DavidB]

Yeh I'm running mine now at feed 1200 and G01 retract at F15000. LOL

[Newbeeee™]

So I just opened 7 using an X5 'doner file' and imported the new up-issued model into it.

Progged away and ran (ubvs) verify and it took out a corner.

Ran (old stylee) backplot and ok.

Watched verify through and saw a dog-leg.

Looked in ops manager>properties>files>and the machine definition was for the X5 file (x5 machine def).

I clicked and loaded the X7mmd and re-ran verify and all was sweet (as X7 machine def is set as per previous posts here ie straight line).

Soooooo, me thinks we need to have a Settings>configuration> switch to 'load latest machine def on opening' (or something like this).

I know it was previously beat about a couple of years ago but it would have saved me a bit of head scratching and time.

[kool]

Just came across little issue with dogleg rapids move for drilling cycles in X7 verify.

 

It looks to me when you are drilling multiple holes in one drilling operation, X7 verify does not show dogleg moves between those holes.

 

I see that in drilling only.

 

Is that a bug, Please confirm!