v bit overall cut depth.

[Boatguy1979]

Is there a way to adjust the overall cut depth of a vcarve v bit. I do not want a flat depth I want the angled look of the regular vcarve but need it to not cut as deep. I hope this makes sense.

thanks
Keith

[mtylerfl]

Hi Keith,

The depth of cut for vcarving (closed vectors), is (automatically) determined by the angle of v-bit you are using and the width inside/between your closed vectors.

Using a 90-degree v-bit will cut shallower than a 60-degree v-bit, for example.

[Rcnewcomb]

Is there a way to adjust the overall cut depth of a vcarve v bit. I do not want a flat depth

Your choices are:
1. Use a bit with a larger angle i,e, 60° rather than a 45°, a 120° rather than a 90°
2. In the areas where you want a shallower cut edit the vectors to be closer together using node editing.

[OneShortPlank]

Hi all,

Complete newbie here with a related question on v-carve toolpath depths.

I made two cuts yesterday using identical workpieces. The file just had the name of one of my kids and a decorative leaf on either side of the name. I copied the file and put my other kid's name in the second file. All the settings were identical. i used a touch probe to zero the work both times. I used the same 60 degree bit. But one of the files was cut deeper than the other cut. The difference is quite visible and significant enough that I would feel comfortable inlaying one with a brass/resin mix as planned, but not the other - it's too shallow.

I've checked the tool settings on each g-code file, the position and thickness of the two workpieces, etc. and can't find any difference between the two set-ups. The font size is the same (I measured the height of the letters and they are consistent).

I'd be grateful for any thoughts on how this might have happened...!

Many thanks,

Alan

[mtylerfl]

Hi Alan,

We need a little more to go on.

At the very least, some photos could help. Can you upload your project (crv) files so we can see how you did your layout and Toolpaths? That would be ideal to have the actual crv files to inspect. (NOT your gcode files)
.

[Rcnewcomb]

Instructions: How do I upload files or photos to the forum?
If the file is too large to upload here you can place it on a site like drive.google.com, dropbox.com, or onedrive.com.
Make the file shareable, and then provide the link to the file here.

[OneShortPlank]

Hi Michael and Randall,

Thanks so much for your help. I'm attching the CRV files here and will try to get a couple of photos just now also.

Thanks again,

Alan

[OneShortPlank]

Hi again,

I'm attaching a photo of the two cuts together here. Hopefully the difference is visible - I'm not sure how well you can see it but hopefully it will give you an idea.

Many thanks again for any ideas you might have,

Alan

[scottp55]

Just to save other people some time maybe;
Alan has set up to Z at material top
I changed text to curves and small "a" is identical size/font/options for both(see pics below).
Hovering over VCarve toolpath...max depth is identical at 6.339mm

Alan,
I can't see any reason in the file for the depth difference.
Therefor (before finishing first cuppa anyways) there must have been something in your Z-Zeroing...
flatness of material...different spot you used for Z-Zeroing...or spoilboard flatness..
or different clamping (pressure maybe).

Doesn't appear to be anything in the files I can see.
What method of Z-Zeroing are you using?
Was your Z-Zero spot on the material At the names?

That's all I can think of at the moment
scott

[OneShortPlank]

Hi Scott,

Many thanks for taking a look - much appreciated.

I used a touch probe to set the z-zero on both. It sits on the corner of the workpiece (top left as you would look at the workpiece if reading the text; bottom left as oriented in VCarve). Maybe I should be setting the z-zero in the centre above the workpiece?

Both pieces were identical in flatness and held down with double-sided tape in the exact same position - I have a corner clamp that I can screw down into t-nuts so that the position is repeatable.

The spoilboard is not flat though - I have been trying to tram the router spindle but haven't been able to do this succussfully yet. However, I thought that with all other settings identical, if the spoilboard wasn't perfect, any resulting error would appear on both workpieces?

By the way, should I be converting text to curves before generating the toolpath?

Thanks again for having a look at this. Hope you've had the first cuppa by now! I'm on number 4...

Alan

[OneShortPlank]

I forgot to ask - would it be advisable to run the file again using something like a 15 degree v-bit to get some extra depth but still keep within the outline of the vector? Is there a risk that I could mess it up?

Thanks!

[scottp55]

Alan,
After looking at closeups of the pic,and ruling out the file..
The best I can figure is "Martha" had a very slight warp up,
And "Adam" had a very slight warp down? (It REALLY doesn't take much!)
Things Look evenly cut from side to side, and top to bottom...
and looking at the 2 pass cuts it doesn't appear to be to far out of tram.
It's Much more important to have a recently skimmed spoilboard,and have material setting uniformly
and Firmly setting on the spoilboard.
I use fences/wedges/cam clamps almost all the time, and always beat down material to the spoilboard with a deadblow on a piece of softer wood after it's clamped.
I Always check bottom of material for gaps/unevenness afterwards...
as even a small chip of wood can throw you off.
The most perfectly jointed piece of wood won't cut well if spoilboard isn't FLAT.

Yes...generally it's best to Z-Zero AT the critical cut because of variances.
I've had pieces that were machine flattened parallel and carved...
then a few weeks later had to carve a dedication on the back in tiny font, and had to Z-Zero
on Each font site on a 24" board. Seen some carvings where people had to Z-Zero each LETTER.

It's generally best Not to convert to curves, as then you can't use the font tools, AND the program won't recognize it as a font. And on cursives and script fonts can lead to issues.
IF you have to convert to curves for Node Edits and such, then usually best to copy after all font tools have been used to a separate layer and then if it gets mucked up...you don't have to start from scratch.
The only reason I converted was to measure an identical single letter for size.

Hmmm....General rule of thumb is that once it's unclamped....all bets are Off!
That's why I always inspect the cut(unless I space it! ), as many things can be fixed or made better
while the board is still clamped.
For instance on yours, you could have cheated Z-Zero down by hairs until perfectly matched
(or used a Start Depth).
As far as rejigging it absolutely perfectly and identically....chances for mucking it up are Big!

Just an example, but I carved a base for a 3D Ural Squirrel on a wormy piece of walnut branch for a nephew. Dedicated the back to him, and took his name down over a bad cell connection.
(he lives 3,000 miles away and only met the 10 yr old twice...and he was always "Nico")
Double live edge and wasn't really a problem until my Mom came to pick it up for shipping...
and said "Where's the "s"??"

I went into the file and placed a single "s"...

Then CAREFULLY aligned the piece with machinist's square, tightened clamps,tap tapped until aligned.
tightened again...rinsed and repeated for almost an hour until piece was down Solid!

Then using tip of 30* engraving bit and nudging by thousandths got lined up with a defined corner of the last letter....and changed my X,Y Zeroes to match reality to the file.

I Z-Zeroed At the letter...then cheated my Z-Zero up .2" so I could Nudge X,Y again by thousandths.
Then carved down(inspected/nudged) in increments to match the existing font.
It was ALMOST perfect, so on last cut Nudged Z-Zero down .005"....
and that Tiny bit, changed it from almost perfect to "Noticeable"

So "MAYBE" worth a shot if "Adam" is not usable for epoxy/brass(??).
Don't think I would go more than a 30 degree.

But I consider my set up very repeatable(if I have two good edges),
and in two tries failed once with very small artifacts from the original carve.
IF I surfaced wood down a smidge, odds got up to 3 out of four good cuts.

Originally was going to say that after assembly....carefully sand Martha to match Adam...
But since Adam may be unusable...that's no good

Hope any of this helps.
Sorry to take so long responding,
scott

[OneShortPlank]

Scott,

Thanks so much for the comprehensive reply! Greatly appreciated. And thanks also for sharing your own adventures - who knew that CNCing can also help you to get to know your extended family better (or at least learn their names!).

Thanks for the tip about tramming. I guess my primary reason for wanting to get it reasonably well trammed is that I can then run another surfacing pass on the spoilboard to get that properly flat. The first pass that I ran has left it very 'ridgy'.

I was hoping to cut some clamps after getting the spoilboard flat - I'm sure if I do a search on the forum here there'll be plenty of suggested designs and maybe a few files available.

I thought maybe that using the touch probe would have guaranteed that it would cut the file again in the exact same posiiton, but I'll take your words of warning on that! I might just cut my losses and forget about the brass inlay this time.

Thanks again for all your help - I'm sure I'll back for more sage advice as I get into this more and more over the coming months...

All the best,

Alan