V-Engrave Plugin

[sraney]

Great Plugin. But I seem to have found an odd issue with memory while generating the toolpaths.  I've pulled the parts apart and reviewed them and can not see a problem with it.

VEngrave7 (Polyline182) is the first one I located. I have even pulled it into a new file and attempted to just generate tool paths for it.  VEngrave15 (Polyline186) also produces the same issue.



 I've attached the CB file

[EddyCurrent]

VEngrave15 works fine for me but 7 takes longer then I care to wait, in fact I did not see it complete.
Also there is no MOP for Polyline (182)
I cut the Polyline (186) into two pieces and each half completed no problem, can't see why it's no good as one line.

[pixelmaker]

hello
first use the -> edit -> polyline -> arc fit with value 0.01 to reduce the nodes.
Then I create a new active layer
Select Polyline 186 and use -> edit -> polyline -> remove overlaps with value 0.01
A new polyline (1) is created at the new layer
Use this polyline (1)  in VEngrave7 without problems.

If you work with dirty files you have to clean the polylines first.

ralf

[pstemari]

Sorry I didn't see this earlier.  Been busy with other things and my engraving project was interrupted by a change of product logo at work.

Yes, the circle is an edge case and I haven't added any code to explicit support it.  There's some optimizations applied to the g-code that remove superfluous points from the toolpath, basically duplicates or points that lie within a tolerance of the line between adjacent points.  What that means for a circle is that all the points are duplicates and get optimized away (good), but that the one remaining point is tossed out (not good).

I'll take a look to see what's involved with a fix.  I don't know off-hand if the remaining point is getting thrown out by my code or CamBam's code.

As far as i18n goes, I don't have any code to explicitly support it.  If anything is happening at all, it's because of underlying support in CamBam. 

[pstemari]

Circles: http://code.google.com/p/v-engrave-plugin/issues/detail?id=20
i18n: http://code.google.com/p/v-engrave-plugin/issues/detail?id=21

I'll also be moving the project over to GitHub sometime in the next few weeks; I will keep you all posted on that.

Tip diameter:  v-bits normally have a small flat on the end.  If you don't adjust for this all the engraving will be too wide by the diameter of the tip.  On a small engraving bit that becomes very important:  0.005" on a 0.010" wide line is pretty noticeable!  On routers making big signs in wood, just set it to zero and don't worry about it.

I like the angle adjustment for depth.  The issue I was struggling with for doing multiple passes was how to make a smooth final pass and avoid any steps.  The angle adjustment just applies a scale factor to the depth, and you can cut, for example, starting 20% of full depth, and then step up to 100%.

[Bubba]

I like the angle adjustment for depth.  The issue I was struggling with for doing multiple passes was how to make a smooth final pass and avoid any steps.
===================
Would it possible to have a maximum depth option (selection) so user can simply measure the bit flute length and determine the depth of the cut? On deeper cuts in wood I don't see as a problem with minimal step. Something it can easily be dealt with. I have used your plugin couple times and job always come out as expected. Nicely done! Thanks.

[pstemari]

It's there, but it's implied by the tool diameter.  The max depth is 1/2*(tool diameter - tool tip diameter)*cot(V-Angle / 2).

In other words, it won't ever plunge past the tool diameter. 

[Bubba]

It's there, but it's implied by the tool diameter.
++++++++++++++++++

OK, I didn't know that. Thanks.

[elf]

Attached are two .cb files. The first, L_Font.cb, is based on a TrueType font, the second, L_Inkscape.cb, on the same font converted to lines and arcs using Inkscape. 

V-Engrave appears to generate the correct toolpath in L_Font.cb but doesn't in L_Inkscape.cb.  What changes do I need to make for V-Engrave to generate the correct toolpath in L_Inkscape.cb?

[Bubba]

convert it to 'region' first. It does work fine here.

[elf]

Thanks, that works.  Now to figure out what the settings will be for the inlay piece

[ajayre]

I've tried cutting the outside of the letter 'C' and at one point the v-engrave path deviates from the curve of the letter. See the screenshot.

The problem isn't a display issue because CutViewer shows the same defect.

Any ideas on how to fix it?

Thanks, Andy

[ajayre]

How can I get the VCarve Pro effect shown in this image?



By using V-engrave on a region and the pocketing the region with a suitable roughing clearance the attached image is the closest that I have come, but this method leaves a plateau on top of the letter.

Thanks, Andy

[blowlamp]

How can I get the VCarve Pro effect shown in this image?



By using V-engrave on a region and the pocketing the region with a suitable roughing clearance the attached image is the closest that I have come, but this method leaves a plateau on top of the letter.

Thanks, Andy

I don't think you can use the current V-Engrave plugin to get this effect.

The Profile MOP does a fair job if you use a truncated cone cutter and run it around the outside of the character (Tool Diameter set to equal the truncated diameter), whilst specifying a Cut Depth large enough for the central ridge to form. This method doesn't give the sharp inner corners to certain letters (E, F, K, etc) that a dedicated Prism MOP would give, but it's still pretty good.


Martin.

[pixelmaker]

hello,
you can make this also with the v-engrave plugin.
You need the letter, you draw a second polyline with the offset function and a third polyline with the half of the distance of the first offset.
The letter and the first offset line you convert in to a region. After you use STR+U on this region.
To cut "inside" the letter you set the stock surface lower then the stock. As lower you set the stock as more you cut to the middle of the letter.
The second polyline with the half distance you need for the pocket.
In the attached file you see how I do this.
You need a cutter with a flat v-angle and a large diameter.

ralf