CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
April 04, 2020, 00:17:20 am


Login with username, password and session length


Pages: [1]
  Print  
Author Topic: G83Extended High Speed Asymmetrical Parametric File Converter  (Read 447 times)
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1291


View Profile
« on: December 23, 2019, 07:39:07 am »

Here is a Plugin That extends the capabilities of the standard G83 Deep Pecking Cycle

It was tested with CamBam ver1.0 rc2.
G83 Extended Pecking Cycles in the plugin menu.

It was Inspired by this video From Hass:https://www.youtube.com/watch?v=AM6nVgKjBQo

If you watch the video, the variables will make sense as it's based on that video.
It was tested with Mach3 and Mach3+cutviewer,Linuxcnc, and the Default PP.
And is for any controller that will accept a G83 code. Not grbl though for obvious
reasons.

The output file is Identical to the input file with only the G83's changed.

The zip file has a Folder that contains the “G83 Default TestFile 1.cb” plugin.dll and the Default setup file.

Unzip the folder to your usual cnc files folder.

Open up the folder and load the cb file then Immediately Save it (this sets the file associations).
I'm using the Default PP and the standard mm libs for the sake of compatibility but you can use
one of the of the above  tested  PP's .

The file has threes mops with the same target depth and different Drill Diameters.
3mm,6mm,and 9mm Drill Diameters and a Target Depth of -30.

Why? because the math works out nicely to show the proportional Asymmetrical thing
so 'for the love of mike' DO NOT CHANGE ANYTHING IN THE FILE'.
Leave it Metric and if you click on the mops and CB asks you to change anything click no.
I've already hard coded the Drill Diameters into those mops in the file.

So now you have loaded up the CB file and saved it:
Now Generate the code ctrl+w or from the drop down menu.

You now have this file:“G83 Default TestFile 1.nc”

Your screen should look like pic1. If you have programmers notepad.
if you are using the windows notepad then your Gcode formatting will be a little different (not as neat).

Now it's time to run the plugin (If you have it already open then you MUST close it and reopen it).
Your screen should look like pic2.

An Important thing to note is that if you adjust the mops in CB then you must re-generate the
Gcode file, as the plugin works with that.

Dave


* Pic 1.PNG (122.82 KB, 1365x729 - viewed 33 times.)

* Pic 2.PNG (198.68 KB, 1365x739 - viewed 38 times.)
* G83 tests.zip (86.68 KB - downloaded 20 times.)
Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1291


View Profile
« Reply #1 on: December 23, 2019, 07:41:42 am »

OK, so to make our first modifications to the G83's output in the Gcode file, we load up the .nc file into the plugin Pic 3.

The plugin should look like this, both the Load .nc file button and the convert button will turn green.
Pic4


An Important thing to note is that if there are Three G83's in the file, then you have to set the variables for each of mops the first time a new file is loaded up, as you start the Iterative process of designing your Pecking Cycle .
For purposes of this example select each of the mop in the drop down box and press the set individual mop settings button.
Pic 5

OK so now we can convert the file (the convert button) has turned green.
Pic 6
Now load up the 'G83 Default TestFile 1 G83Extended.nc'  file that has now been produced with
preferably with Programmers Notepad .


* Pic 3.PNG (34.34 KB, 793x297 - viewed 29 times.)

* Pic 4.PNG (72.27 KB, 693x575 - viewed 34 times.)

* Pic 5.PNG (2.12 KB, 307x43 - viewed 30 times.)

* Pic 6.PNG (4.61 KB, 311x107 - viewed 32 times.)
Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1291


View Profile
« Reply #2 on: December 23, 2019, 07:45:18 am »

Why? Because it knows when the file has been altered by the plugin so when you click on the 
Programmers Notepad to have a look at your new file It will ask you to reload the file.
Windows Notepad won't do this so you have to remember to do this. This can cause the error
of converting a file but nothing seemingly happens, it has of course your just looking at 'Yesterdays News'.

The G83's in the file that you have produced should look Identical to the ones on the posted
called 'G83 Default TestFile 1 G83Extended compare this file to the one you just made.nc'
If all is well you are good to go.

For Designing you also want to click the Output Comments Check Box.


1. The Stock size 25 mm x 25 mm mild steel bar stock.
2. The Target Depth of the hole will be Z-30 mm as this is a through hole and we
want the cutting edges of the drill to pass below the bottom of the stock.
3. This a Ten times the Drill Diameter Deep Hole. X10

There are seemingly a lot of variables to fiddle with, this provides get flexibility in
designing the G83 but can be confusing to start out, so well start out with a simple clearance
move to be performed at Z-18 mm (6 Drill Diameters).


* Pic 7.PNG (27.99 KB, 796x447 - viewed 30 times.)
Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1291


View Profile
« Reply #3 on: December 23, 2019, 07:48:22 am »

Then to make the change active for the mop click on the Set Individual Settings Button
(It'll turn Green)  then click the convert button, Now open the file with Programmers Notepad.
When you examine the Gcode, You'll see that  a Chip Clearance Move has been created at Z-18.
in Pic 7

Too move the Clearance move Up or Down in the Hole  all you do is change the variable,
so say we want to lower the  Chip Clearance Move from now Z-18 to Z-24 then we would with a 3 mm tool
add 2 Drill Diameters to the variable now(6) and make it (Cool 8 x 3 = 24. you can
work this out with the number being in  Drawing Units by pressing the 'calc' button.
So for this example file this is mm (24mm).

Remember that if you make a change to any of the settings you have to press the
Set Settings button for that mop again and then press convert.
The clearance move has now moved from  Z-18 to Z-24
Pic 8

Now you are ready for the 'Rinse and Repeat' part, move the  Clearance move Up or Down
by adjusting the Chip Clearance Move  text box value then click the set settings button and
then convert button and examine your file by clicking on  Programmers Notepad in the task
bar and it will ask if you if you want to reload the file click yes.


* Pic 7.PNG (27.99 KB, 796x447 - viewed 29 times.)

* Pic 8.PNG (19.31 KB, 527x394 - viewed 32 times.)
Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1291


View Profile
« Reply #4 on: December 23, 2019, 07:49:57 am »


When I get a bit more time I'll do the 'Stay inside Hole' and Return to Clearance Plane check boxes.
 It's fairly simple, you just have to know that in practice  you want to keep this variables minimum
value to  at least 'Half a drill diameter' to ensure the cutting edges stay completely under the stock surface.

To Illustrate one  of the powers of parametric programming of the pecking cycle look at 9 metric  and 10 which is in inches with measurements close enough to the 3mm Z-30 hole X10 .
I used a one eighth drill in a inch and a quarter hole.
Pic 9
pic 10

Notice that I have not made any to changes the variables in the plugin to get a functionally equivalent pecking cycle across the two measurement systems because they are both X10 holes.
Merry Xmas
Dave


* Pic 9.PNG (74.5 KB, 680x575 - viewed 30 times.)

* pic10 .PNG (150.73 KB, 1116x700 - viewed 35 times.)
Logged
Bubba
CNC Jedi
*****
Offline Offline

Posts: 2870



View Profile
« Reply #5 on: December 23, 2019, 14:03:09 pm »

Although I haven tried this plugin yet, I appreciate your effort. Thank you, and Have Merry Christmas.
Logged

My 2¢

Win 10 64 bit, CB [1.0} rc 1 64 bit, Mach3, ESS, G540
Pages: [1]
  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 0.131 seconds with 19 queries.

Copyright © 2018 HexRay Ltd. | Sitemap