"Clearance" problem in Mastercam 2018

[Matt Berube at Ferron Mold]

I am using 2-D toolpaths (face, contour) and I have "clearance" checked in Linking Parameters with an Absolute value of 2.0 

"Use only at the start and end of the operation" is not checked.

Ignoring the settings above, Mastercam is only using the clearance value at the beginning and end of the operation.  All other moves are only retracting to the "Retract" plane.

Is this broken in 2018? Anybody else having this difficulty? 

[crazy^millman]

24 minutes ago, Matt Berube at Ferron Mold said:

I am using 2-D toolpaths (face, contour) and I have "clearance" checked in Linking Parameters with an Absolute value of 2.0 

"Use only at the start and end of the operation" is not checked.

Ignoring the settings above, Mastercam is only using the clearance value at the beginning and end of the operation.  All other moves are only retracting to the "Retract" plane.

Is this broken in 2018? Anybody else having this difficulty? 

Sorry I am not following you?

Is what specifically broken? What you described is the behavior I would expect to see. Are you saying you or you don't see the behavior? If you don't what do you specifically see that is wrong? If you do then what changed from previous version to 2018 that is giving you specific problems?

[Matt Berube at Ferron Mold]

Sorry I wasn't clear enough CM

Check out this file if you have a minute.

I expect 2.0 CLEARANCE moves throughout this operation but they are only happening at the beginning and end.

 

clearance problem.mcam

[jeff]

UN-check retract should make it do what you want.

[huskermcdoogle]

Matt,

Yup, I would call that broken as well.  I noticed that myself the other day.  It is certainly not functioning as it once did.  What I do to get around it at this point is uncheck retract.  Then it will retract to clearance everytime, with more efficient code.

I would report it as a bug.

[crazy^millman]

6 minutes ago, huskermcdoogle said:

Matt,

Yup, I would call that broken as well.  I noticed that myself the other day.  It is certainly not functioning as it once did.  What I do to get around it at this point is uncheck retract.  Then it will retract to clearance everytime, with more efficient code.

I would report it as a bug.

I reported this back when 2018 1st came out and yes it does not act the same as before, but like you mentioned it is more efficient of a toolpath. I cannot remember if I got a bug number or if I was told now the software acts like it is supposed to. When you have over 3400 emails to and from CNC Software over the years hard to keep track of what conversation is what.

[Matt Berube at Ferron Mold]

I sent it up to QC.  I'll update here when they respond.

[gcode]

Its still broken in MC2019

[crazy^millman]

1 hour ago, gcode said:

Its still broken in MC2019

Broken or working as designed?

[Matt Berube at Ferron Mold]

10 minutes ago, C^Millman said:

Broken or working as designed?

As designed, apparently.

Here's the official (very speedy too!) response from QC.

"I tested in X9 and 2017 and 2018 is working the same way X9 and 2017 worked.
If you want the tool to go to the 2” clearance plane, uncheck Retract."

 

[crazy^millman]

8 minutes ago, Matt Berube at Ferron Mold said:

As designed, apparently.

Here's the official (very speedy too!) response from QC.

"I tested in X9 and 2017 and 2018 is working the same way X9 and 2017 worked.
If you want the tool to go to the 2” clearance plane, uncheck Retract."

 

Then since Mastercam's inception they always did it wrong and finally got it right about the X9 release? Okay good to know it was being used wrong for all those years.

Like when Quickmask went from Right and Left click to only Left Click for 2017. Wrong for years?

Like the Unselect all removed from the selection bar wrong for all those years?

[Colin Gilchrist]

6 minutes ago, C^Millman said:

Then since Mastercam's inception they always did it wrong and finally got it right about the X9 release? Okay good to know it was being used wrong for all those years.

Like when Quickmask went from Right and Left click to only Left Click for 2017. Wrong for years?

Like the Unselect all removed from the selection bar wrong for all those years?

It's "Microsoft's" way, or the highway apparently.

The removal of Left-Click/Right-Click for the quickmasks really sucked. I strongly dislike the divided diagonal button approach.

[huskermcdoogle]

59 minutes ago, Matt Berube at Ferron Mold said:

As designed, apparently.

Here's the official (very speedy too!) response from QC.

"I tested in X9 and 2017 and 2018 is working the same way X9 and 2017 worked.
If you want the tool to go to the 2” clearance plane, uncheck Retract."

My Response would have been, "then why have a checkbox for retract only at start and end of operation"

[crazy^millman]

16 minutes ago, huskermcdoogle said:

My Response would have been, "then why have a checkbox for retract only at start and end of operation"

That is just for you have certain abilities with that and not the ability to use it as it says it is to be used since the software is not designed to do it that way now.

[nickbe10]

2 hours ago, Matt Berube at Ferron Mold said:

"I tested in X9 and 2017 and 2018 is working the same way X9 and 2017 worked.
If you want the tool to go to the 2” clearance plane, uncheck Retract."

I'm running X9 and the check box works to restrict clearance to start and end, when Retract is checked. Of course it won't work if  Retract is unchecked.......

And as for Colin's comment about the MS way I agree with C

[Matt Berube at Ferron Mold]

1 hour ago, huskermcdoogle said:

My Response would have been, "then why have a checkbox for retract only at start and end of operation"

I was close to asking that too but after testing myself, I think I figured out why.

My example file had just 1 pocket.  It seems that Mastercam's specification is that within a single contour, the RETRACT value is used.  If you were to take my example file and delete the chain I have in the operation and then draw 2 rectangles and chain both of them, you will see the different output depending upon whether the box is checked or not.  

Basically, within a single contour, you will get the retract.  With more than 1 contour, you'll get the retract within each contour but then the clearance will be used when traveling between contour #1 and contour #2.  

[navsENG]

I've noticed this too. I thought I was doing something wrong because I was out of programming for about 2 years.. Came back and am on X9..

Was wondering if maybe I just forgot and was doing it the wrong way, lol. As others have stated, un-checking the box works.

[Leon82]

I do a part with 3 1mm slots around a 10mm hole which create a clamp.

I check use clearance only at start and finish.

There are a total of 6 chains and I have depth cuts at .005 and sort by depth. I set the retract to -.005 incremental. And top of stock to incremental also. Maybe -.005 but I can't remember.and feed plane the same.

 

The end result it. 2.0 clearance and the tool stays down and rapids between each slot. I chained it so it will rapid clear of material. 

 

So I would play with some of the settings.

[Slepydremr]

I was searching and found this thread. It sort of touches on the problem we have, only since we program parts in aircraft coordinates the retracts are really jacked up if you select by depth. This is in 2018 and 2019.

 

Anyone know if this has been addressed in 2020. I've found that submitting tickets does nothing but get me told to wait for the next release.

I've got some screen shots and a file, but for whatever reason it's not letting me attach them.

[Slepydremr]

retracts.mcam

[nickbe10]

1 hour ago, Slepydremr said:

It sort of touches on the problem we have, only since we program parts in aircraft coordinates

I worked at a shop where we did that (admittedly this was back in X4) and I wasn't very impressed. Even 4 axis programs were unstable in holding their selected origin, which if you are on a constructed WCS will instantly throw your retracts off in either absolute or incremental, and with multi axis you lost considerable functionality if you were not on MC zero.

Of course the whole reason for doing it is that when there is a Rev change the new model should come in in the same position. In the 4 years that I was there I was able to take advantage of this 0 (zero) times. These days Rev changes in aircraft are usually non dimensional , however most of my programs in those days included multi axis toolpaths so unless I moved to MC zero I lost significant functionality. So I constructed 3D translate axis on a level to be able to get the part in position quickly.....never needed that either. Still not convinced of the efficacy of machining in airplane space.....I know people do it all the time......just not convinced its not more trouble than its worth.

[Slepydremr]

We've been programming in WCS since it came out in Mastecam 9.1    All 3, 4, and 5 axis. Some functionality doesn't work correctly, never has, but most things work fine.

We have a customer that likes to move pilot holes quite often, super fast to bring in the new model and then move the holes without having to re-orient the parts and make sure it was moved just right. When true position is .007" you better have moved the new part to the exact spot the other one was at.

We also do a fair amount of spares parts for the gov, most of those old parts have loft surfaces in space, then you have to model the part around that. We keep it in aircraft coordinates for inspection purposes. 

Modeling up parts with drawings from the 50's and spreadsheets of space point to define some loft surface out in space is awesome.

[jlw™]

I reported this the first time in 2017.  Then in 2018 and 2019.  CNC said and it seemed to be corrected in 2020 but I just got it TODAY.

I usually set my clearance plane to what I want my retract to be and then use ref points for clearance Z.  That workaround gives basically the exact tool path every time I use it.

[Jayson Kramer]

Just tested in MC 2020 B4 and works as expected now.

[jlw™]

22 hours ago, Jayson Kramer-CNC Software said:

Just tested in MC 2020 B4 and works as expected now.

Yeah, I have literally seen it twice in all of 2020.  Unfortunately it was about 300 ops deep in a file.