CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
November 16, 2018, 13:29:48 pm


Login with username, password and session length


Pages: [1] 2
  Print  
Author Topic: Inverting the Z-Axis  (Read 844 times)
Incomple
CNC Ewok
*
Offline Offline

Posts: 41


View Profile
« on: July 05, 2018, 21:55:49 pm »

Hello Everybody,
I have a bit of an odd request; I'll start by disclosing that I need a work-around for some circumstances that are beyond my control.
Here's the situation: I use CamBam at home and I LOVE it.  Separate from my home hobby machine, there's a 3-axis machine at work that I don't control; but I'm allowed to use after hours with the shop foreman's permission.  I may not change any settings on that machine, or else the day-shift crew might not be able to use the machine in the manner to which they've become accustomed later on.  I changed a setting once and lost access to the machine for months; the foreman still doesn't like it when I come poking around his area.
Anyhow... the machine comes bundled with CAM software that's very buggy and can't generate toolpaths that are appropriate for my application.  These are toolpaths/G-code that CamBam generates with ease.  Earlier today, I called the machine's manufacturer and asked if it was possible to feed the machine G-Code that had been generated with software other than what comes bundled with their machine.  To my surprise, there was a method!  I ran home over lunch, generated a simple .nc file, and brought it back with me to work.  I had daydreams of getting CamBam at work and freeing the guys that work with this machine from the confines of the software that they use now (they've all told me that they hate their current CAM software.)
I just fed the CamBam generated G-Code to this 3-axis machine, and it seemed to work as I had hoped.... with one big exception.  The machine interprets Z-movements differently than I do.  The machine expects Z0 to be at the surface of the stock, POSITIVE Z commands plunge into the stock and NEGATIVE Z commands retract the cutter away from the stock.  When I'd finished, the only cuts into the material with the clearance "retract" commands that are supposed to pull the cutter out/away from the material.
Right or wrong, it's opposite of my personal interpretation, but that's what the machine does.  I called the machine's mfg to see if there was a setting that I could flip when I was using the machine (no luck.)  So it looks like my only option is to ask CamBam to generate G-Code that matches the expectations of this machine.  Is it possible to have CamBam output G-Code that "inverts" Z-directions? 
I hope that there is.  My section at work could really use this machine, and we don't have the $$ or space to get our own CNC for our specific application.  Just to re-iterate; I may only feed this machine G-Code, I can't change any settings on the machine (aside from current workpiece origin) or the software that drives the machine.
Any help would be appreciated!!
Thanks!
Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5214



View Profile WWW
« Reply #1 on: July 05, 2018, 22:19:45 pm »

Hello

I think it's not possible only with the post pro settings, but certainly it can be done with a post treatment of the Gcode ?

If I well understand the only thing to do is to replace all Z negative values in the Gcode by positive and vice versa  ?

What is the PP you are using for this machine ? I've a post treatment skeleton that I can adapt to your PP, currently it modify X value, but I can easily modify it so it modify Z

++
David
« Last Edit: July 05, 2018, 22:26:02 pm by dh42 » Logged
10bulls
Administrator
CNC Jedi
*****
Offline Offline

Posts: 2097


Coding Jedi


View Profile WWW
« Reply #2 on: July 05, 2018, 22:44:00 pm »

This should be possible in the post processor.

Attached is a copy of the Default post processor, with all {$_z} values replaced with {$_zneg}.
Copy this into the cambam system\post folder, then restart CamBam.
Select this post in your machining properties.

To modify your own post processor, just go through all the 'Moves' and 'Canned Cycles' properties and
wherever you see {$_z} change it to {$_zneg}

I haven't tested this much myself, so please double check everything first.
I'd hate for your foreman to put you on the CNC naughty step again because of me!  Grin


* Default-InverseZ.cbpp (1.1 KB - downloaded 15 times.)
Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5214



View Profile WWW
« Reply #3 on: July 05, 2018, 22:55:54 pm »

Hello Andy

Ah yes, the {$_zneg} ... I totally forgot it ...  Embarrassed

++
David
Logged
Incomple
CNC Ewok
*
Offline Offline

Posts: 41


View Profile
« Reply #4 on: July 05, 2018, 23:13:32 pm »

You guys are great!! I'll give it a shot and let you know how it works!!
Logged
Incomple
CNC Ewok
*
Offline Offline

Posts: 41


View Profile
« Reply #5 on: July 06, 2018, 22:36:16 pm »

Feedback: Guys, that worked GREAT!!
Just finished my work day; I managed to pop into our machine shop and run some CamBam-generated G-Code.  The stuff that was generated with your recommended post processor tweaks worked great!
The spindle speed didn't take, but I can adjust that manually from the machine's control pendant.  I can live with that.

I am just thrilled; I love CamBam, and now it looks like I might be able to use it to solve problems at work!

Which brings me to my next question...  I work for a big company that has a lot of rules.  One of those rules is that regular computer users never have "admin rights" on their machines.  If admin rights are required, then an IT professional will either visit your machine personally or remote in and perform whatever task requires the rights.

So, if I wanted to use CamBam at work, would this lack of regular admin rights be a problem?  I seem to remember CamBam asking me to "run as administrator" a few times.  Not a big deal for a hobbyist, but I fear that I might hit a wall if it requires permissions that are restricted by my employer.

Do you think I might run into issues or am I worried about nothing?  I'm not a network/computer security guru.  I'd hate to make my employer buy a few licenses and then be unable to use them because of admin rights.
Hope this question doesn't sound too naive... like I said, this is a subject in which I'm just a novice.
Logged
10bulls
Administrator
CNC Jedi
*****
Offline Offline

Posts: 2097


Coding Jedi


View Profile WWW
« Reply #6 on: July 07, 2018, 00:12:22 am »

Yay! I hope you have much success with your machines!

CamBam mostly only needs admin permissions to run in evaluation mode, or when entering a license key.
If there is a license file detected in the CamBam program folder, normal user rights are OK.

However, the user will also need write access to the CamBam system folder, which on most Windows is located...
C:\ProgramData\CamBam plus 0.9.8\
or
C:\ProgramData\CamBam plus 1.0\
for the latest development version.

The installer will set this permission (if run as admin) or for V1, it should prompt for admin permission to grant this  the first time CamBam is run.
V1 may also need admin permissions for Tools - set file associations (but this just need setting once per user).
If your IT guys have any questions, I am happy to help... I was one for a number of years and remember the funny handshake and everything!  Wink
Logged
10bulls
Administrator
CNC Jedi
*****
Offline Offline

Posts: 2097


Coding Jedi


View Profile WWW
« Reply #7 on: July 07, 2018, 00:36:10 am »

The spindle speed didn't take, but I can adjust that manually from the machine's control pendant.  I can live with that.
If you have any sample gcode that works for that machine, or a programming manual, it may be possible to set the spindle speed in the post processor definition.
Logged
Incomple
CNC Ewok
*
Offline Offline

Posts: 41


View Profile
« Reply #8 on: July 11, 2018, 20:03:25 pm »

If you have any sample gcode that works for that machine, or a programming manual, it may be possible to set the spindle speed in the post processor definition.

I will see what I can find!


Next question!  I'm working through the process of having CamBam added to my employer's approved software list.  When the time for purchasing licenses comes; how is large-organization licensing handled?  One license per user?  One license per machine on which CamBam is installed?  One license per shop? etc.
Thanks!
Logged
10bulls
Administrator
CNC Jedi
*****
Offline Offline

Posts: 2097


Coding Jedi


View Profile WWW
« Reply #9 on: July 11, 2018, 22:53:13 pm »

Next question!  I'm working through the process of having CamBam added to my employer's approved software list.  When the time for purchasing licenses comes; how is large-organization licensing handled?  One license per user?  One license per machine on which CamBam is installed?  One license per shop? etc.
Thanks!
For commercial use, we request one license per 'concurrent' user, that is the number of people typically using CamBam.

You are welcome to copy your license to multiple machines for convenience.

If you have more than 5 users we can organise a site license.  There are a couple of different options here, so if you think this would be preferable, please email 'support @ cambamcnc.com' (no spaces) or use the contact form at http://cambamcnc.com/contact and we will provide further details.

Thank you and I hope this help!
Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7638



View Profile
« Reply #10 on: July 11, 2018, 23:46:27 pm »

Andy, the concept of "concurrent users" is fair and equitable.  Thank you for your good service to our community!

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
jim1108
Droid
**
Offline Offline

Posts: 81


View Profile
« Reply #11 on: July 13, 2018, 12:23:46 pm »

Hello everyone,
   I was curious if inverting the A axis just like the Z axis as above would have the same affect?

My machine’s 4th axis rotates CW for positive A moves and CCW for A negative moves.

Whenever I wrap a drawing around the circumference of a part, text for instance, it comes out inverted and backwards. So, I have to draw in normally, then rotate and mirror it in Cad before importing it into CB.

This would save the trouble of doing the footwork in Cad.

Maybe adding a mirror A axis feature for the  post processor?

I am not at work today, so I cannot experiment with it.


Logged
Dragonfly
CNC Jedi
*****
Offline Offline

Posts: 2036



View Profile
« Reply #12 on: July 13, 2018, 12:28:21 pm »

If you are using Mach3 (or any other controller which allows output signals configuration) it can be done by changing the active state of the 'dir' signal.
Can also be done in hardware by swapping the ends of one of the motor coils.
Logged

Before asking a question do some effort and walk through all menus and options in CamBam.  Maybe the answer is there. Please.
jim1108
Droid
**
Offline Offline

Posts: 81


View Profile
« Reply #13 on: July 13, 2018, 12:35:55 pm »

Hello Dragonfly,

I am running a Daewoo DMV6025 with a Fanuc 16-iM control.

It’s an old machine, but very rigid. We have it anchored in a cement footing.

The control does allow me to mirror any axis in the settings, but I have to remember to change it back for my regular jobs.

I was just trying to eliminate the extra drawing and/or settings changes by having the post take care of it.
Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5214



View Profile WWW
« Reply #14 on: July 13, 2018, 21:02:57 pm »

Hello

Quote
  I was curious if inverting the A axis just like the Z axis as above would have the same affect?

I do some tests ; Gcode is wrapped with the Wrapper plugin.

To revert the A axis, you can use a xneg or yneg instead of of the regular x and y macros (using aneg has no effect, because it's X or Y that is converted to A)

Another way is to check or uncheck the Reverse angle box in the Wrapper plugin.

++
David


* wrapper.jpg (56.17 KB, 979x650 - viewed 25 times.)

* wrapper_invert.jpg (56.62 KB, 831x656 - viewed 26 times.)
Logged
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 0.153 seconds with 20 queries.

Copyright © 2018 HexRay Ltd. | Sitemap