I want to vcarve a few words in a piece of plywood. Made pockets of 5 mm on shapestrings, and in Path made a vcarve job with start depth of 19.04 mm, and final depth of 14.04 mm.
But when I brought the job to the CNC, it appeared the depth of the characters was for the most only about one mm.
Inspecting the gcode, I found the Z-value stayed at about 18 mm, and not, what I would expect, 14.04 mm
I want to carve a few words in piece of plywood. I’ve made shapestrings in Draft, and pocketed them 5mm deep in Part Design. Then, in Path, made a VCarve job, with start depth of 19.04, and final depth of 14.0.
Milling that out on the cnc, the carving came out only about 1mm deep.
Inspecting the gcode, it appeared the lowest Z-value was around 17.5 mm, while I would expect 14 mm, the final depth
Unfortunately, I can’t provide the FCStd-file (to big) r gcode (extension not accepted; but also of little use without the .FCStd-file I would think.)
Any one an idea what goes wrong here, and how to overcome it?
hello,
without a file it is difficult to answer, the possibilities are numerous and vary, it can come from the cam or the controller, check your G-code to see if it comes from the cam (shapestrings incorrectly positioned in Z, origin piece, incorrectly positioned.. …)or a controller problem with a reference 0 of the engraving tool incorrectly positioned…
You’re right, but I did not man to crosspost, but a few hours after I posted it the first time, I got the message that this post was not found. So I presumed it was vanished some way, and posted the topic again…
I attached a test piece, with the same heights and depths as used in the problematic piece.
The gcode generated also shows that the desired depth of 14.04 mm as never reached.
I created a test piece this morning, with the same heights and depths of the problematic piece. It shows he same problem.
I have attached the resulting FCStd file in the above posting.
To summarize:
the height of the plywood is 19.04 mm
the shapestrings are also positioned at Z=19.04
and then pocketed 5 mm deep
the vcarve job has a start depth of 19.04, and a final depth of 14.04
but the resulting gcode has a depth which is at it’s minimum 17.334, where I would expect 14.04
Hope this clarifies what the problem is, or at least, what my problem is.
Attached is an excerpt of the gcode, in .csv-format. Only the G1 commands listed, with an extra column (S) for the step number, and sorted by Z-position.
Toggle on the visibility of the tool. Then inspect the operation and find a line of gcode corresponding to an interesting segment. It will position the tool at that point.
It looks like it’s operating correctly. The tool is going down until it hits the sides of the pocket.
2024-01-26_09-53.png
Hmm, I think I see your point. But, in defining the carving operation, I select the bottom of the character as the base geometry, not its sides. So I would expect that the tool is going down until the bottom is reached. That in that process the sides of the character are a bit widened is - for the result I want, at least - of no importance.
If the way I create this job is not right, what is?
Thanks for your reaction! (A phrase not added in all my replies, but I’m grateful for everyone who takes the trouble of looking in to the problems I have.)
That’s not the way the vcarve works. It respects the boundary of the character and calculates the depth to achieve that. The final depth is the maximum that the cutter will plunge, even if the V doesn’t reach the sides of the glyph. As far as I know, that’s how v-carving works in general.
Ah, now I see what happens, thanks! Problem is that this behaviour is absolutely not what I want. I want a constant depth, defined by the depth of the pocket. And with a slope in the form of the tool used. That the (top of the) sides widen, so be it, no problem. So the algorithm should - in my case - not respect the boundaries of the character, but the given depth.
I’m having a hard time imagining how the result would be anything other than terrible. Do you have an image of a cut that was done successfully this way (in any software)? Maybe I’m still misunderstanding.
Things you could try:
Lie to the software about what kind of tool you have. Define a V- bit with an extreme angle ~1-2 degrees so that it always fits into the pocket.
Hand edit the gcode and substitute all the Z values for the maximum depth.
Or you could copy the v-carve operation code and start hacking on it.
If I understand what you want, I have done it successfully. I wanted to cut text with sloping edges to the letters, where the top of the letter would be wider than the bottom. In FreeCAD I defined a Pocket operation, with a 1/16" straight endmill. Then at the CNC I instead used a cheap 3/8" V-bit which has a small flat at the tip instead of coming to a sharp point. Depth of cut was only 0.8mm. I determined the depth of cut by doing test cuts in cheap material until I was happy with the results.
Good day.
Attached is one possible solution that might be in line with your goal. This solution will not produce a flat bottomed letter, but will have a maximum depth of approximately the 14.04 mm you desire. The solution presented is more a proof of concept. All I did was make a copy of the original VCarve operation, calculate the difference between the bottom of the original operation cut and your desired 14.04 mm Final Depth, which is about -3.29 mm (I used a script function I have to identify the ZMin value of the original VCarve path). I then changed the Z placement value on the copied operation to this -3.29mm. Done. However, this creates a -3.29 stepdown that might be too great for your setup. If this is the case, use the same copy/placement-adjustment combination to create additional intermediate step cuts.
If you desire a flat bottom for each letter, then this method will not serve that purpose. A different approach will need to be used.
Cordially,
Russell
OS: Windows 10 build 19045
Word size of FreeCAD: 64-bit
Version: 0.22.0dev.35735 (Git)
Build type: Release
Branch: main
Hash: c12a5c2a163c1a277cf273106899209792be152d
Python 3.10.13, Qt 5.15.8, Coin 4.0.2, Vtk 9.2.6, OCC 7.6.3
Locale: English/United States (en_US)
Installed mods:
* FC_SU
* freecad.gears 1.0.0
* freecad.pathred
* Z_MacroStartup
Eventually, I decided to take a simple approach: set the Z=0 at a slightly lower (0,5mm) lower than the real zero. This way the characters get enough depth to let them stand out (or in, if you want…) satisfactory, and yet behold the form prescribed by the typeface.
The characters are too small to do a cut with a straight endmill, would take plm. 0.3 mm I think.