CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
December 14, 2019, 21:43:43 pm


Login with username, password and session length


Pages: [1] 2
  Print  
Author Topic: [1-49] Weird Engrave Issue Using Work Offsets G54 & G55  (Read 2017 times)
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3818


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« on: November 03, 2019, 23:15:20 pm »

Making two parts at a time one set of operations is to making an engraving on a surface about 0.9 inches below zero.  The lines are projected to the surface.  

There are two sets of operations.  One set is an exact copy of the other set except that the first set has G55 in the MOP Header and the other set has G54 in the MOP header.  

The first set (doesn't mater which set is ordered to cut first) rapids down to depth and then plunges a very small amount to engrave the lines.  The second set goes to depth at the programmed plunge feed rate instead.  If I reverse the order of operations the result is the same.  The first set to execute rapids to depth and the second set travels to depth at plunge feed rate.  

Its a complex engraving and takes about 19 minutes to engrave if it works properly.  The second set of operations takes over an hour.  That pretty significant.  If I was only making two units it would be no big deal.  The job would be done and I would have shipped it them already.  Unfortunately (or fortunately for my bank account) I am making 50 of them.  

I CAN NOT upload the file.  Its proprietary customer information.  I also tried to duplicate the problem with a sample file, but it didn't exhibit the problem.  

I'm at a loss as to what caused the problem.

For now my solution is to cut the entire job except the engraving, and then great two engraving files to be executed sequentially after the main file.  I have to select a file and press start three times, but its still faster than the way it was behaving when all part of the same code file.  

Video showing issues:  https://youtu.be/EO-CYX71Ohs

« Last Edit: November 04, 2019, 01:00:34 am by dh42 » Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3818


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #1 on: November 03, 2019, 23:18:48 pm »

I suppose another alternative is to add the .NC file for the G54 Engrave and the G55 Engrave back into the CamBam file.  Its a work around, but the problem itself is so weird. 
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5677



View Profile WWW
« Reply #2 on: November 04, 2019, 00:58:15 am »

Hello Bob

If I well understand, it's the "Fast Plunge Height" that is not working for the second engraving MOP ?

I've done some tests and even without G54-55 I fall on strange results with the fast plunge height. and they are not consistent.

Not sure it is related to your problem ... but there is something wrong somewhere  Shocked

Example: I set "Fast plunge height" to 2 in the machining folder

I set a profile mop on a simple rectangle with TD = -1 clearance plane = 10 , stock surface = 0 DI =3
(default PP used)

in the Gcode I get:

G0 Z10.0
( T5 : 3.0 )
T5 M6
( Contour1 )
G17
M3 S12500
G0 X-29.1087 Y-31.8052
G0 Z4.0 'should be 2 for stock surface = 0 and FPH = 2
G1 F600.0 Z-1.0

now if I change "Fast plunge height" to 4 in the machining folder, with the same other settings I get

G0 Z10.0
( T5 : 3.0 )
T5 M6
( Contour1 )
G17
M3 S12500
G0 X-29.1087 Y-31.8052
G0 Z6.0 'should be 4 for stock surface = 0 and FPH = 4
G1 F600.0 Z-1.0

more strange, If I set stock surface to 3 in the mop, and with 4 in fast plug height, I get 3+4 = 7 for the plunge, so it's OK .... but ... the cut depth is not right and is Z=0 instead Z=-1 ..

G0 Z10.0
( T5 : 3.0 )
T5 M6
( Contour1 )
G17
M3 S12500
G0 X-29.1087 Y-31.8052
G0 Z7.0 'OK SS=3 + FPH=4 > Z = 7
G1 F600.0 Z0.0 'wrong, must be -1
G1 F800.0 Y27.167

The value for the plunge seems always be 2 units more than expected in this case.

It seems also dependent of the depth increment ; a DI =0 gives the right values for plunge and target depth ... other values gives wrong plunge height but not always wrong target depth ....

Also depending of the target depth, sometime it works OK, sometimes not ...

The problem is the same with CB 0.98 and 1.0 RC3

++
David

« Last Edit: November 04, 2019, 01:15:33 am by dh42 » Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1171


View Profile
« Reply #3 on: November 04, 2019, 04:23:58 am »

CB's ok, and it's nothing to do with the offset's.

This behavior happens when you have inadvertently set the "Fast Plunge Height"  to a height above the Clearance Plane Height, in which case the code is omitted in the Gcode file, else if you set the "Depth Increment" greater than your target depth then you get the behavior that David gets in the first example.

Dave


* Depth Increment greater than target depth.PNG (51.1 KB, 630x427 - viewed 26 times.)

* Depth Increment less than target depth.PNG (67.77 KB, 759x480 - viewed 31 times.)

* fast plunge height set to 2 clearance plane to 3.PNG (37.48 KB, 619x345 - viewed 31 times.)

* fast plunge height set to 4 clearance plane to 3.PNG (44.33 KB, 674x381 - viewed 31 times.)
Logged
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3818


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #4 on: November 04, 2019, 04:43:00 am »

Clearance is .05.  Fast plunge is -1. 
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5677



View Profile WWW
« Reply #5 on: November 04, 2019, 05:11:48 am »

Clearance is .05.  Fast plunge is -1. 

-1 = automatic setting = one minor unit of the grid. (0.0625" if you're using the default grid settings)

++
David


Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1171


View Profile
« Reply #6 on: November 04, 2019, 06:20:52 am »

Bob, for sure you have an incorrect setting in the Mop, I made this rubbish 3d mop with the stock surface above the target depth.
What CB does here is insert the Depth Increment above Z0  a safe move.
There are interdependent variables in the mop, DI,CP,SS,TG which all effect the outcome.
If you could at least get an example CB file posted, I have some analytical tools that I made for a newer version (not posted here) of the Quantum Eraser that will find those kind of errors in moments not months.

Dave


* 3D mop stock surface error.PNG (37.08 KB, 603x323 - viewed 28 times.)
Logged
Dragonfly
CNC Jedi
*****
Offline Offline

Posts: 2224



View Profile
« Reply #7 on: November 04, 2019, 07:59:34 am »

I am seeing this oddity on regular bases and not only in the case described by Bob.
For example - multi level pockets. Sometimes (and I can't find a repeatable cause) the tool lifts to clearance and then goes down at plunge speed, i.e. very slowly. G0 to FPH (dynamically calculated when material is removed) is missing. Maybe, just maybe, it happens when lead-in is set to 'Spiral'.
With spiral drill when two consecutive drill MOPs a defined on one hole - one rough, one to finish diameter - after the first drill and lifting to clearance the tool is moved slowly at plunge speed to the center of the hole, then back to offset from center and then plunge to FPH is usually done with G0.
With pockets I suspect that the method of alternating start points for each level (which I definitely dislike because it brings unpredictability) may also have an impact on the code generation with missing fast plunge.
Didn't bother to report it 'cause, as I have said, I can't identify a repeatable reason.
Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1171


View Profile
« Reply #8 on: November 04, 2019, 10:37:17 am »

Quote
With spiral drill when two consecutive drill MOPs a defined on one hole - one rough, one to finish diameter - after the first drill and lifting to clearance the tool is moved slowly at plunge speed to the center of the hole, then back to offset from center and then plunge to FPH is usually done with G0.

I made a file like this and have posted it so where all on the same page.
It's your max cross over distance, set to zero when this happens. see the code in the pic's.
For this one I can reproduce your result and the remedy is easy, If you come across a problem in the future, post it and
I'll run it through the QE tool and see what it says.
I suspect this may be what's wrong with bobs file. but we have not got enough information to go on.

Dave

Logged
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3818


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #9 on: November 04, 2019, 14:06:56 pm »

I think you missed the part where it works perfectly in the first set of operations and does not work in the second set of operations and both sets of operations are identical except for the application of a work offset in the header.  Also as described in the first post. Either set of operations works perfectly when executed stand alone. No changes are made in the mops.
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
Garyhlucas
CNC Jedi
*****
Offline Offline

Posts: 1314


View Profile
« Reply #10 on: November 04, 2019, 17:55:27 pm »

Bob,
Is all of the G-code from the G50 and G55 code on identical? Occasionally on Mach 3 if I do a feedhold and restart I get the spindle moving at plunge speed not at feed rate. When the program reaches the next feed rate change it goes back to normal operation.
Logged

Gary H. Lucas

Have you read my blog?
 http://a-little-business.blogspot.com/
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3818


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #11 on: November 04, 2019, 19:57:45 pm »

This is not a Mach 3 bug.  CamBam is actually creating different code even though the MOPs are identical. 

I have looked at the g-code, and in the first set it shows a rapid (G0) to about .05 above the projected lines then plunge (G01) to the cut depth.  In the second set there is a G01 from clearance height to cut height. 

If you looked in my video (sorry my microphone failed) you can see Mach 3 shows red rapids for the first set of operations and blue tool paths for the second set. 
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3818


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #12 on: November 04, 2019, 21:22:00 pm »

I think you missed the part where it works perfectly in the first set of operations and does not work in the second set of operations and both sets of operations are identical except for the application of a work offset in the header.  Also as described in the first post. Either set of operations works perfectly when executed created stand alone. No changes are made in the mops.

Sorry, should have said created.  Not executed. 
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1171


View Profile
« Reply #13 on: November 04, 2019, 22:29:57 pm »

Quote
I think you missed the part where it works perfectly in the first set of operations and does not work in the second set of operations and both sets of operations are identical except for the application of a work offset in the header.  Also as described in the first post. Either set of operations works perfectly when executed stand alone. No changes are made in the mops.

No I didn't miss any of the the points you made, I specifically made the CB file (which no one downloaded) I posted, mimic the behavior you described.

You can deselect the first two spiral drilling mops and get different code as opposed to having them all on and with no G5X's in sight.
It's simple either your mops need tweaking or the geometry needs checking again. I found no issues in using the offsets or not. I simulated everything.

Bob I've had some problem files,which I'd given up on in frustration, only to open it up a few weeks later and spot the error almost immediately, I must have looked at that particular mop many times previously and saw nothing.

Without a example file demonstrating the error we are just speculating and can go no further.

Dave
Logged
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3818


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #14 on: November 05, 2019, 01:49:39 am »

Well for now I am running three code files for the job.  25 done.  25  more to go.  Then I get to machine the back side.  LOL. 
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
Pages: [1] 2
  Print  
 
Jump to:  

Powered by MySQL Powered by PHP Powered by SMF 1.1.21 | SMF © 2015, Simple Machines

Valid XHTML 1.0! Valid CSS! Dilber MC Theme by HarzeM
Page created in 0.135 seconds with 19 queries.

Copyright © 2018 HexRay Ltd. | Sitemap