Author Topic: V-Engrave Plugin  (Read 162790 times)

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 4739
    • View Profile
Re: V-Engrave Plugin
« Reply #285 on: April 20, 2021, 21:46:07 pm »
David,

I compiled it for "Any CPU" so it should work on 32 and 64bit.
Tested on 64bit but I do not have a 32bit version installed to test it on that.
Made in England

Offline dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 6489
    • View Profile
    • Cambam V1.0 French Doc
Re: V-Engrave Plugin
« Reply #286 on: April 20, 2021, 21:53:30 pm »
Thank Eddy,

Seems to work well on 32bits too ;)

++
David

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 4739
    • View Profile
Re: V-Engrave Plugin - Now with Depth Increment
« Reply #287 on: July 22, 2021, 08:13:55 am »
Please test the attached version 13 of the plugin.

1. Removed the code that was originally there for testing purposes, just to streamline things a bit. They can always be added back in if required.
2. Added a Depth Increment parameter.

Notes:
I'ts best to leave "Max Depth" at the default value of "positive infinity"
Set Depth Incement to a required value.
If Depth Increment is set to a value that far exceeds the expected depth then the plugin will produce one toolpath at full depth.
( Shoud I make it so that if "Depth Increment = 0" this means go to full depth without any increments ? )

Toolpaths will be created at each depth increment step then a final pass at full depth.

When simulated, you will observe that the plugin follows the outline rather than going down the middle, this is intentional and what we have understood about it's operation for a while.

Please report any issues then once deemed to be acceptable I will post the updated source files.

As an alternative method please also have a look at the plugin by GeoffreyGRoy; https://cambamcnc.com/forum/index.php?topic=9228.msg72057#msg72057

Edit: please see a more recent post for the latest version
« Last Edit: July 26, 2021, 18:45:09 pm by EddyCurrent »
Made in England

Offline GeoffreyGRoy

  • Storm Trooper
  • ***
  • Posts: 234
    • View Profile
Re: V-Engrave Plugin
« Reply #288 on: July 22, 2021, 09:03:45 am »
Dear Eddy

Many thanks, this is what we have been waiting for!  I will test it out.
Geoff

Offline Bubba

  • CNC Jedi
  • *****
  • Posts: 3145
    • View Profile
Re: V-Engrave Plugin
« Reply #289 on: July 22, 2021, 13:51:27 pm »
Thank you Eddy,

I will test it out as soon as start to feel better. Currently fighting terrible head cold.

Be safe.
My 2¢

Win10 (64 bit, CB(1.0)rc 1(64 bit) Mach3, ESS, G540, Endurance Laser.

Offline Bubba

  • CNC Jedi
  • *****
  • Posts: 3145
    • View Profile
Re: V-Engrave Plugin
« Reply #290 on: July 22, 2021, 14:54:24 pm »
Just finished testing it by running the gcode generated in simulator. It does how Eddy described, even though it does not control the max depth (what I'm interested in)is still maybe useful to some..
My 2¢

Win10 (64 bit, CB(1.0)rc 1(64 bit) Mach3, ESS, G540, Endurance Laser.

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 4739
    • View Profile
Re: V-Engrave Plugin
« Reply #291 on: July 22, 2021, 15:01:36 pm »
To control max depth you should set the "Max Depth" parameter to something other than "positive infinity", e.g. 1/2" then set Depth Increment to say, 1/8" if you need that facility.

It would not however produce something like you showed with Artcam and it would have to be a total rewrite of the plugin to do something like that, assuming someone knows how.
« Last Edit: July 22, 2021, 15:07:39 pm by EddyCurrent »
Made in England

Offline Bubba

  • CNC Jedi
  • *****
  • Posts: 3145
    • View Profile
Re: V-Engrave Plugin
« Reply #292 on: July 22, 2021, 16:03:48 pm »
I have tried the Max depth and it throws error. Anyway, thank you for the explanation.
My 2¢

Win10 (64 bit, CB(1.0)rc 1(64 bit) Mach3, ESS, G540, Endurance Laser.

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 4739
    • View Profile
Re: V-Engrave Plugin
« Reply #293 on: July 22, 2021, 17:22:26 pm »
Bubba,

Setting Max Depth works fine and always has, please attach a file that throws an error.
 In any case do not use negative numbers, both parameters need POSITIVE numbers., that's not my doing, the plugin has always required that.

As you know the plugin plunges a V tool to a depth that is calculated from the width of the gap it's cutting, e.g. the inside of a text character.
Max Depth defaults to positive infinity as a way to give "unlimited" freedom to the tool with regard to depth of cut.

Let's try some numbers;

Example 1.

Depth Increment = 0.05"
Max Depth = 0.5"
The calculated maximum depth that the tool needs to go in order to produce the required cut = 0.25

The result will be 5 passes of 0.05 to reach a depth of 0.25"
Max Depth will be ignored because the calculated tool depth does not go that far.

Example 2.

Depth Increment = 0.05"
Max Depth = 0.1"
The calculated maximum depth that the tool needs to go in order to produce the required cut = 0.25

The result will be 2 passes of 0.05 to reach a depth of 0.1"
The calculated tool depth will be ignored because Max Depth prevents it.
« Last Edit: July 22, 2021, 17:30:10 pm by EddyCurrent »
Made in England

Offline dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 6489
    • View Profile
    • Cambam V1.0 French Doc
Re: V-Engrave Plugin
« Reply #294 on: July 22, 2021, 17:42:30 pm »
Hello

Thanks Eddy  ;D

Not yet tested, but how about the  "Max Depth" set to Auto (this calculate the max depth so the tools never go below the V, to avoid cutting with the shank)

https://cambamcnc.com/forum/index.php?topic=7910.msg63327#msg63327

is this the same result that using the last Geoff's "step engrave" plugin ? (also not yet tested)

++
David

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 4739
    • View Profile
Re: V-Engrave Plugin
« Reply #295 on: July 22, 2021, 17:58:02 pm »
David,

Setting Max Depth to "Auto" seems to work but I can see some code changes would be required. The modifications I made actually write a value into MaxDepth but I did not take account of "Auto"

Geoff's plugin uses a different idea and the results may not look identical.

Edit:

This is how Auto is calculated;

Code: [Select]
private double ComputeAutoMaxDepth()
        {
            if (ToolDiameter.Cached <= 0)
            {
                return double.PositiveInfinity;
            }
            return 0.5 * (ToolDiameter.Cached - ToolTipDiameter.Cached) / Math.Tan(0.5 * ToolVAngle.Cached * DEGREES);
        }
« Last Edit: July 22, 2021, 18:21:01 pm by EddyCurrent »
Made in England

Offline dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 6489
    • View Profile
    • Cambam V1.0 French Doc
Re: V-Engrave Plugin
« Reply #296 on: July 22, 2021, 19:31:11 pm »
Quote
The modifications I made actually write a value into MaxDepth

It is a good thing, because the Auto setting is very useful but it did not give any feedback of what the max depth value will be used, And when we must to know this value, it is necessary to "convert toolpath to geometries" and then to use the "object extrema" on the toolpaths to find it.

nice job  ;D

++
David

Offline Bubba

  • CNC Jedi
  • *****
  • Posts: 3145
    • View Profile
Re: V-Engrave Plugin
« Reply #297 on: July 23, 2021, 12:29:32 pm »
Setting Max Depth works fine and always has,
*******************
Removed the V13 after test because I don't have reason to keep it, and after put in the 'old' plugin in its place tried the Max Depth again. It does work fine as long numbers are used as Eddy suggested. Now, if I could convert the tool pats to geometry and use pocket MOP it would be the answer I'm looking for.

Edited: Found it in the V-Engrave MOP... Don't get old, folks.. :-[
« Last Edit: July 23, 2021, 23:35:09 pm by Bubba »
My 2¢

Win10 (64 bit, CB(1.0)rc 1(64 bit) Mach3, ESS, G540, Endurance Laser.

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 4739
    • View Profile
Re: V-Engrave Plugin
« Reply #298 on: July 23, 2021, 14:01:29 pm »
Bubba, it must be the heat  ;D 

There is very little difference between v12 and v13 of the plugin, there was no need or benefit changing back to v12.

How is toolpaths to geometry going to help you ? I'm interested to know your thoughts on this.
Made in England

Offline Bubba

  • CNC Jedi
  • *****
  • Posts: 3145
    • View Profile
Re: V-Engrave Plugin
« Reply #299 on: July 23, 2021, 21:41:41 pm »
How is toolpaths to geometry going to help you ? I'm interested to know your thoughts on this.
********************************
Eddy,
Glad you asked.
After converting the created toolpath to geometry, deleted unneeded lines to create pockets. It take a bit of work, but it is worth the effort considering that few times in the past I needed to carve 6 inch bold text letters in 1 inch thick board. It would take large V cutter and very deep cut which I want to avoid for various reasons. By controling the depth I can get away with thinner board and often smaller diameter cutter. First MOP (V-Engrave) is done with V-60 at .187" depth, the second MOP(pocket) is done with the same tool but with different tool number (created tool #60 with diameter 0.01" ). I haven't tested  on real wood but it does look promising on simulator.

My 2¢

Win10 (64 bit, CB(1.0)rc 1(64 bit) Mach3, ESS, G540, Endurance Laser.