V-Engrave Plugin

[GeoffreyGRoy]

Dear David

Well, that makes it simple - never to told to learn new tricks!
Geoff

[EddyCurrent]

Geoff,

With this information, my issue is really just about setting the "Depth Increment" to 0.0, I think I am suggesting that for consistency with V12 a Depth Increment of 0.0 with a Max Depth of Infinity should give the same result in v14 (and not go into an infinite loop).

I've got that fixed now

On another question: If you use "Tool Paths to Geometry" for the generated tool Paths the order of the polylines is not always "correct" , i.e. not in "increasing max depth" order as one might expect - particularly if you intend to use the new Polylines to create an Engrave MOP.

The toolpaths are added to a toolpath sequence in what I thought was the correct order, it seems to work correctly like that but have not tried it as you mention. I shall probably pass on that unless I see the toolpaths going wrong.

I am also not sure whether it might also be useful to consider modifying the Max Depth values so they are consistent with all (?) other MOPS, i.e with -ve values (for going downwards).  Perhaps open for opinions?

This will be more difficult as the origanl code expects a positive value so I shall leave this to someone else if it is required 

[EddyCurrent]

Please find version 15 attached.

1. If "Depth Incement" = 0 ,  this will be taken as "go immediately to full depth cut". This is the same action that version 12 and previous would take.
2. Selecting "Auto" for "Depth Increment" will set it to zero.
3. Parameters for "Depth Increment" and "Max Depth" must be positive numbers. If negative numbers are used then the affected option will be flagged as "Error"
4. As David requested the "Auto" value for "Max Depth" will be shown in the bottom Message Log Window.

I have also attached the source code project files for Visual Studio.

Unless there is some serious defect I think that's me done with this for now. 

Edit: I updated the version number shown on the Form as detected by Geoff.

[Bubba]

Thanks Eddy,

 As always nice job. Even though I just finished testing the earlier version I'm sure those results are the same with this one. I was going to report the plugin did excellent job.
Using file "TEST 1278"as test, created the V-varve toolpaths and converted one of those using toolpath to geometry. It is used (after little editing) for pocket MOP. Very happy with the result.

Thanks again.

[EddyCurrent]

Bubba,

I thought it would be easier using the alternative method with an offset line as I described earlier.

[Bubba]

Eddy,

I don't understand what do you mean by offset method, wouldn't it create a step? Sorry for being thick headed.

The attached picture illustrate exactly what it look like, and that's how artcam does it, except all of this is done in one MOP using the same tool.

[dh42]

all of this is done in one MOP using the same tool.

Not sure it's a good idea to machine the flat regions with a V tool, the flat surfaces will not be very smooth I think ... 

++
David

[GeoffreyGRoy]

Dear Eddy

Many thanks for the updates to V15.

On the order of the Polylines in "Toolpaths to Geometry" I am attaching an example with the problem.  The generated geometry is in Layer1.  If you look at the order of the Polylines in the last 'f' (27, 28,29,30) you will see that, 27 has a max depth of -7.1, 28 has a max depth of -6, 29 has  max depth of -4 and 30 has a max depth of -2.  Normally 27 would be cut first!. 

Note that some of the letters have the correct order.

Also, the version number on the About popup needs updating.

thanks

Geoff

[Bubba]

all of this is done in one MOP using the same tool.

Not sure it's a good idea to machine the flat regions with a V tool, the flat surfaces will not be very smooth I think ... 

++
David

David,
I know, but... Before V-Engrave was available as plugin I was using artcam (very old version)for V-engraving and it does have option for controlled depth of cut. It does all with the same tool, and the finish is acceptable, considering the type of tool used. Now, if you want smooth finish this option should be avoided, or use very small router bit. I'm to lazy to change tools, and happy to live with this finish, sand it little bit, and use gel stain, then multiple coats of spar urethane and call it good. BTW, the picture attached to my previous post is out of the artcam simulator, it is pretty accurate.

[Dragonfly]

David,
I know, but... Before V-Engrave was available as plugin I was using artcam (very old version)for V-engraving and it does have option for controlled depth of cut. It does all with the same tool, and the finish is acceptable, considering the type of tool used. Now, if you want smooth finish this option should be avoided, or use very small router bit. I'm to lazy to change tools, and happy to live with this finish, sand it little bit, and use gel stain, then multiple coats of spar urethane and call it good. BTW, the picture attached to my previous post is out of the artcam simulator, it is pretty accurate.

First of all I must admit I lost track of V-Engrave development.
But I think Bubba is right based on his experience. The same approach is used by another very popular commercial program - V-Carve by Vectric. What's more both ArtCam and V-Carve can work with V-cutters that have a flat tip and can do side stepping (a kind of pocket) until they reach the top surface boundary of a shape when the DOC is limited or the tool's full possible depth is not wide enough. IMHO in the majority of cases a single V-cutter usage is the preferable approach. Especially on small lettering and ornaments.
Using a larger tool for removing flat areas is better only for areas large enough to allow for a flat cutter with large enough diameter to make it possible to cut fast.
For example if I use a V-cutter with 0.5 mm flat tip using a 0.8 mm end mill is not appropriate as it will break being much more weak than a V-shaped tool.

[EddyCurrent]

Eddy,

I don't understand what do you mean by offset method, wouldn't it create a step? Sorry for being thick headed.

Bubba, I described it here; https://cambamcnc.com/forum/index.php?topic=3513.msg72169#msg72169


Geoff,

Thanks for the test file.

Edit:

Geoff,

Form version number updated, thanks for spotting that.

The toolpaths are not like normal where the tool cuts to a particular depth first, the tool changes Z to acommodate the geometry and to fit the point of the V tool into tight corners.
There is a method in there called, "DetermineCuttingOrder", it uses various optimisation modes so you could have a go at trying different optimisation modes in the MOP settings.
Also with "Regions" it looks like the outer lines are processed before the inner ones so the tool may go to full depth for the outer lines then rise again to do the inner ones.

Failing that, feel free to have a play with the code. 

[Bubba]

Eddy, Sorry those results are not the same, at least for me they are not.  It's OK though, I'm happy with what I got so far.

Cheers..

[GeoffreyGRoy]

Dear Eddie

It seems that if Optimisation mode is set to "None" then the order of the cutting paths is correct.  I have tried to update the code to force this for the MOP, but I cannot recompile it as I get a number of error messages, see attachment, that refer to copying files to the "D" drive - I do not have one, and I have been unable to locate the settings in the VS project that might fix this - any thoughts?

I would think that it is straight forward to force None optimisation as the default - to be safe.

Geoff

[GeoffreyGRoy]

OK, I found the problem in the .csproj file.  I don't understand why I couldn't find it in the VS properties - I will now take a look at the code.
Geoff

[EddyCurrent]

Geoff,

Too late, I've attached the latest version, Optimisation set to "None", thanks for testing this.

Those errors stem from the "References" section in VS, you have to set the path to CamBam's dll's there.

I have also attached the updated source project files.

Edit: If you open an old V-Engrave cb file it already has Optimisation Mode set to whatever it was when the file was saved so you should manually set it to "None"
If however you start a new cb file and insert a new V-Engrave MOP it will be automatically set to Optimisation = "None"