Open Source V-Carving

[WillAdams]

I haven't found a technique for converting an svg to dxf which retains curves and is easily installed on my machine.

I'm also more familiar w/ graphic design tools than CNC.

I'd be glad of a step-by-step solution to this.

[scorch]

Inkscape is an open source design tool not a CNC tool.

From the Inkscape web Page:

What is Inkscape?

Inkscape is an open-source vector graphics editor similar to Adobe Illustrator, Corel Draw, Freehand, or Xara X. What sets Inkscape apart is its use of Scalable Vector Graphics (SVG), an open XML-based W3C standard, as the native format.

In order to make a DXF file in Inkscape you just bring open a design in Inkscape as an SVG then select "Save As" and change the output format to DXF.

If any parts of the design are missing in the export you may need to go back and convert the missing features to paths by selecting "Path"-"Object to Paths" from the menu bar. If the SVG includes raster images you can use "Path"-"Trace Bitmap". I my experience you only need to convert text and raster images to paths. Everything else will be exported. Depending on how your software exports text you may not even need to convert the text.

The DXF output uses splines for arcs. I have never looked into how close the splines match up with the original design.

[WillAdams]

F-engrave would be much more useful to me if it had the same sort of type adjustments which Glenn Reid’s nifty TouchType.app for NeXTstep had.

Had a page on that — might still be in the Wayback machine. Members.aol.com/willadams

If you have any interest in GNUstep it’d probably be an interesting project.

I think I’ll have to look into making a front-end using LuaLaTeX and some HyperCard clone.

[eqalizr]

Can you explain where you define the diameter of the straight cutter bit and how do you get the save function to include the straight word in the gcode save function?
I think I have seen some source code that appears to do just that but not sure if it ever gets executed.

[WillAdams]

I believe you’re asking how I did the profile cuts along w/ the V-engravings?

I had to use MakerCAM for the former, creating the cuts in register w/ the engraving. Full workflow more or less:

- draw up design in Macromedia Freehand
- export to .pdf, open in Inkscape, export as three SVG files: fixture, dial and parts w/ duplicated and additional geometry where needed
- use MakerCAM to create G-code for the fixture and parts — latter is broken up into two files, one for mounting holes, the other for the parts
- import the dial into FontForge and export as a .ttf into F-Engrave’s Font directory, process at the correct size to match the fixture and parts
- make the fixture, add suitable hardware, mount the stock, drill mounting holes, engrave dial, cut out parts
- add suitable hardware (one piece required an additional fixture, trimming and flattening another just trimming)

[scorch]

Can you explain where you define the diameter of the straight cutter bit and how do you get the save function to include the straight word in the gcode save function?
I think I have seen some source code that appears to do just that but not sure if it ever gets executed.

There are two types of cuts in the v-carve window that use a straight cutter.

1. At the top of the v-carve window "Straight" cutter can be selected. Using this option will calculate a tool path that cuts just the outline of the design, similar to v-carving but it will miss any sharp corners because it is using a straight bit. When you have "Straight" cutter selected the "V-Bit Diameter" controls the diameter of the straight bit. I see now that this is not clear so I will have the text label update to indicate this fact in the next version.

2. At the bottom of the V-Carve window there is a cleanup section. In this section the cleanup cut diameter is set to the diameter of the straight bit used for cleaning up material inside of the design that was left after a v-carving operation. To save the g-code for the cleanup operations you need to use the "Save Cleanup G-Code" button. When you save the cleanup g-code it will automatically add "_cleanup" to the file name to distinguish the saved file from the main g-code file.

straight_cutter.png


@WillAdams, Clearly you have used Inkscape before so I didn't need to explain to you what it was in my previous post. sorry about the confusion. (Maybe the info will clarify it for someone else )

[WillAdams]

I asked for it.

I'm still curious as to how to get the best possible DXF export from Inkscape --- either I wind up w/ short little line segments, often which aren't properly closed, or it crashes (possibly 'cause I haven't installed a plug-in properly).

[voltsandbolts]

I asked for it.

I'm still curious as to how to get the best possible DXF export from Inkscape --- either I wind up w/ short little line segments, often which aren't properly closed, or it crashes (possibly 'cause I haven't installed a plug-in properly).

I import the dxf into Cut2D and close all of those gaps, they have a setting to join the line segments. I believe some 2D CAD programs can do this aswell.

Sent from my XT1080 using Tapatalk

[scorch]

F-Engrave v1.56 is out with some bug fixes and better line/arc fitting.

There was a huge bug in the old curve fitting which caused the "M" in some fonts to be engraved wrong. This version fixes that and just makes the curve fitting generally better.
The output g-code generated by the new version can be as little as one quarter as many lines of g-code when compared to previous versions.

F-Engrave Download

[scorch]

F-Engrave v1.57 is out with a bug fix for the feed rate.

The feed rate was not being written to the output g-code files in v1.56

F-Engrave Download

[Vogavt]

Thanks for the fix! Truly appreciate your continuing development.

I guess it's just a fluke that the file size for v1.56 and v1.57 is exactly the same.

Opened successfully and states v1.57 right on the top of the bar!

Have you thought about how to handle double entry? I know you can have multiple lines (use that alot) but would be a welcomed addition to be able to place different words with different fonts all in one file. I would also be a welcomed addition to be able to import a dxf/bmp and put text at the bottom, again all on the same screen/file.

A wise man told me once "I'll ask for the moon, even when I know I won't get it, but I'll still settle for a great lump of cheese"!

[scorch]

... would be a welcomed addition to be able to place different words with different fonts all in one file. I would also be a welcomed addition to be able to import a dxf/bmp and put text at the bottom, again all on the same screen/file.

I don't think combining different fonts and/or images will ever be incorporated in F-Engrave. It is probably better to not have those features than to have them poorly implemented. If you need to combine different objects you can always use an external design program like Inkscape and bring the final design in as a DXF file.

[Vogavt]

True. I'm already doing this sort of thing.

Sent from my VS990 using Tapatalk

[gilles1180]

Hi, I'm new to F-engrave, and I find this piece of SW awesome.
I'm interested to understand the internals of the calculations done to determine the radius circle, and being new to the topic (and not english native speaker), I find it hard to grasp. Not so much the calculations, but the fundamentals explained at the beginning. I'm missing where the local coordinate system is placed at the beginning. (x1,y1) and (x2, y2) are the end points of a given step ? I wonder if there is a longer explanation for curious newbies like me.

Also, I found a small bug by accident. I guess it's a corner case but I mention it : put only a "-" in the input text and there will be an error on line 3463 and 5943. I'm using v. 1.57.

[scorch]

To give context to this answer I just want to say that gilles1180 is asking about the F-Engrave V-Carve Calculations page on my web site.

@gilles1180

I will try to explain a little bit.
1) For each line segment the I determine the angle of the line segment then do a coordinate transformation (i.e. rotate the coordinate system mathematically) and translation. so that the current point on the current line segment is located at (x,y)=(0,0) and the second point in the current line segment is to the right of the starting point (0,0). The (0,0) point is labeled in the figures on the v-carve calculations page and the line segment is represented by the red horizontal line in the same figures.

2) For each line line segment in the design or font (except the current one) is checked to determine the resulting radius. Only the smallest radius is kept. During this checking the start and end of each line segment is set to (x1,y1) and (x2,y2) respectively. So x1,y1,x2 and y2 are set for each line segment and checked using the minimum radius calculations. The different figures on the web page show the different special cases that need to be checked.

3) Since the original coding there have been some improvements in the algorithm that increase the speed. The main improvement is that a grid system is set up an it is determined which line segments have influence in each grid section. So when the v-carve calculations are being performed only the line segments that pass through the current grid are checked with the minimum radius calculation.

I hope this helps a little. Feel free to ask again if I missed your question completely.

Also thanks for the bug report. I will look into that and get it fixed for the next release. I recently improved the curve/line fitting and it looks like you have found a case where it fails.

[gilles1180]

Thanks, that helps a lot and I appreciate the time you take to answer. Still 2 questions :

1. I don't understand the following sentence (probably my english). Can you help me?

The calculation is dependant on the font being defined by
loops that are created CW (clockwise). Internal
loops are defined CCW (counter clockwise). If this
convention is reversed the flip normals option in
F-Engrave will correct the calculation.

2. I'm worried that if you have 2 parallel segments (your first particular case) that have a cut of radius R, then in the middle with some types of wood it might degrade the surface and not be clean cut. I would have imagined an R-x with x small being taken to have a bit of margin. Or do I miss something? I'll try it anyway.

Thanks,

Gilles

[scorch]

1. I don't understand the following sentence (probably my english). Can you help me?

The calculation is dependent on the font being defined by
loops that are created CW (clockwise). Internal
loops are defined CCW (counter clockwise). If this
convention is reversed the flip normals option in
F-Engrave will correct the calculation.

F-Engrave follows the each of the paths in the design and cuts to the right side of the path as you follow the path from beginning to end. So if a path is circular and it starts at the top and follows the arc of the circle to the right (like the hand on a clock) then F-Engrave will cut the inside of that circle. If the same circular path is defined starting at the top and following an arc to the left F-Engrave will cut the outside of the circle. The first case is clockwise (CW) and the second case is counter-clockwise (CCW).

F-engrave is smart enough now that it will fix the direction of the paths internally so the input does not need to follow this convention anymore. This statement is still true for the calculations performed inside F-Engrave but the user doesn't need to worry about it anymore.

2. I'm worried that if you have 2 parallel segments (your first particular case) that have a cut of radius R, then in the middle with some types of wood it might degrade the surface and not be clean cut. I would have imagined an R-x with x small being taken to have a bit of margin. Or do I miss something? I'll try it anyway.

I have never had a problem with this. If you want to leave a little extra material you can setup your cutter slightly higher than the surface of the material to be cut. Then there will be a small offset from your deign on all edges.

[gilles1180]

Hi Scorch,

I forgot to thank you for your explanations. Thanks for the great work and putting this in opensource !

Gilles

[cparsons]

I think F-Engrave is an outstanding piece of work - and have been inspired to have a go at doing some engraving, I have a metalworking mill (Sieg SX3) - do you think this would be any good for wood engraving? Looks like you need a lot of speed (top speed on an SX3 is 1700 rpm unmodified) Love the video of the 'Scorch' inlay

Failing that can you suggest a suitable/appropriate bit for aluminium/brass engraving? I would think the 0.1 - 0.3mm V bits would be easy to break? Or worth a try?

Best wishes and thank you so much

Chris

[WillAdams]

I just used some 1/8" Kyocera Carbide V-bits when engraving my locking register calipers: Project Shapeoko