Minimum Vertical Retract

[Jason @ CPM Industries]

Does anyone else seem to have this issue of cutting into the part?

We have all haas machines and it occasionally does it on all of them.

As a default we have it set to Minimum Vertical Retract with rapid move turned off. Part clearance in set to 1 inch.

Most of our jobs are cut in layers so when only cutting the first 3 inches of a 14 inch job

we can't have the machine retracting the full 14 inch every time.

The old style toolpaths would go to the clearance plane you tell it to and ignore the part witch is what we need.

The HS toolpaths go to the hight of the part every time no matter what you put in the clearance plane.

If anyone has seen this or can tell me a way around it that would be great. Thanks

[Jason @ CPM Industries]

This picture shows that cutting with a VMC we have all ready cut the first layer

and have added a second layer. The top of the part is not added yet. How do we stop it from going

above the entire part like we could in the old style toolpaths. The minimum vertical retract occasionally cuts

through the part so that can't me the right choice.

[Pilot Plant Supervisor]

I was told by our re-seller to use Minimum Distance with output feed move checked and set to 500 (IPM) or whatever the machine will allow. That said, I don't use it. Our parts are generally smaller than what you are working on, so I use Full Vertical Retract to save my nerves. When I tried Minimum distance, if I hit feed hold when it gets close to something,the machine decelerates. If there was truly a clearance issue, it could crash before the machine coasts to a stop. I should add that I was using a Haas EC-1600, so it might be more sluggish than a smaller machine.

[Jeremy Herron@DBS Solutions™]

I use it all the time and I have not had a problem with this, was the surface gouged being used as a drive surface?

[Cannon]

It depends how the machine is set up if it will gouge the part at rapid minimum distance. Minimum distance is safe if you use the feed mode but close to vertical walls it still jumps up without any reason..

[Jason @ CPM Industries]

No it was not a check surface and it did not even show up in verify.

[gcode]

if you use minimum vertical retract and G00 rapids, you are going to have a crash

 

you need to set it to G01 rapids and F at the fastest feed rate your machine can run ..

 

that way rapid motion will be in a straight line...

[Cannon]

Mastercam could atleast give a warning about it and not let everybody gouge a part to find about this "feature"

[gcode]

Mastercam could atleast give a warning about it and not let everybody gouge a part to find about this "feature"

 

 

its not a Mastercam problem.. it's a function of how your machine rapids.

Some rapid in a straight line some don't.

Mastercam gives you the ability to handle both conditions.

[Thee Rickster ™]

True, but I am pretty sure most cam packages have the same ailment and it

is also not let know to users.

 

when using, min dist, make sure your part clearance, on the linking parameters

page in the tree is .15" or something like that, and it shouldn't gouge. also if you

'edit common parameters' make sur you dont check absoluteretract and use the same

value as clearance or the "part clearance in (linking parameters) also changes to

that value. on any surfacing tool path

[Cannon]

Mastercam warns me when I open second instance that it may crash my computer, it could do the same thing and warn me when I use minimum retract that I might crash my machine.

BTW I learned it the hard way years ago.

[Thee Rickster ™]

Same here......

[gcode]

it's up the user to know their machine..

 

how can you stand there and watch it run day in and day out and not know if it doglegs??

 

at least in a place like this the programmer has a lame excuse ...

there are 20+ different mills here, some dogleg, some don't

 

I assume they ALL do and act accordingly

[Thee Rickster ™]

coming right off of surfcam, MC bit me with retract clearance(default at .25) when standing cor geometry

is higher then my z-0-. Surfcam doesn't have ludicrous defaults that you have to seek out

 

It come out of the box in safe mode.......

[Cannon]

coming right off of surfcam, MC bit me with retract clearance when standing cor geometry

is higher then my z-0-. Surfcam doesn't have ludicrous defaults that you have to seek out

 

It come out of the box in safe mode.......

 

My favourite in X6 was that all the high speed toolpaths had tooltip defaulted at center. But Im a professional programmer so I should know to look for these

[Jason @ CPM Industries]

if you use minimum vertical retract and G00 rapids, you are going to have a crash

 

you need to set it to G01 rapids and F at the fastest feed rate your machine can run ..

 

that way rapid motion will be in a straight line...

 

Gcode,

By setting my output feed move, that will create all G01 rapids?

[Scott Lundin Shopware Inc.]

Jason,

It will create G01 linear feed rate move that will maintain a straight line without doglegging and hitting the part.

[Guest]

I've explained this before, I should add it to my sig

 

When a machine is in a rapid move, all axis can arrive to the final point at different times, which ever is closer will get there first. So you can get strange moves because as the distance changes the shape of the rapid move will change

 

When in a feed move, all axis' MUST arrive at the final point at the same time. It is a more controlled motion.

 

This is why I NEVER use Minimum retract as a rapid, no system can show you the move

[Thee Rickster ™]

Minimum distance works excellent!

No issues that I can recall

 

Saves on machine wear with those thousands

Of retracts removed.

[gcode]

this is very easy to visualize

 

MDI

 

G00 X0 Y0

X12. Y4.

 

if your machine doglegs it will rapid in a straight line to X4. Y4. then run straight along X to X12.

 

that is dogleg rapiding.

 

If you were deep in a pocket you just smacked a wall even though it looked fine in Backplot or Verify

 

Now do the same thing only

 

G00 X0 Y0

G01 X12. Y4. F300. (or what you machine's max feedrate is)

 

you get a straight run from X0, Y0 to X12 Y4

 

What you see in mastercam is what you get on the machine

 

This is the basics of G01 rapiding as used in Mastercam high speed toolpaths

 

I wish it were available on all the milling toolpaths..

[Jason @ CPM Industries]

Thanks for the feedback everyone. I turned the output feed move on with 300F.

How do you get the feed to stay in the defaults?

I changed it in the defaults then when I write a new toolpath its back to 1000.

[Thee Rickster ™]

Yeah Mc is funny that way,

 

I redid the 500. thing 50 times and nothing, save this reboot that....then gave up.

but i kid you not that it eventually a few weeks later it just starts working.

No idea why or how, but after a month or so mine finally stays at 500.

 

 

Cheers

Rick

[Jason @ CPM Industries]

You would think that would be such an easy fix for MC. Hopefully its in the next update.

[Jason @ CPM Industries]

Does anyone else seem to have this issue of cutting into the part?

We have all haas machines and it occasionally does it on all of them.

As a default we have it set to Minimum Vertical Retract with rapid move turned off. Part clearance in set to 1 inch.

Most of our jobs are cut in layers so when only cutting the first 3 inches of a 14 inch job

we can't have the machine retracting the full 14 inch every time.

The old style toolpaths would go to the clearance plane you tell it to and ignore the part witch is what we need.

The HS toolpaths go to the hight of the part every time no matter what you put in the clearance plane.

If anyone has seen this or can tell me a way around it that would be great. Thanks

 

you have to change your maximun feed rate in machine parameters.