[vpl]

Hello All,
Thank you for taking your time to read this.
I'm trying to make a v carved sign. I have a lot of general cnc routing experience but not much in the sign making area. My issue is when I choose to rough the area before using a v bit tool I have to use the final depth of cut on the v tool. If I don't it won't recognize some of the geometry and on the second pass it will run the bit straight through existing lettering. So if I use a a pocket depth of .250" , I can set the depth of cut on the roughing tool at .125". No problem. It roughs out fine in two passes. If I set the depth of cut on the v tool at .125 it will run through some of the letters on the second cut. If I set the doc on the v tool at .250 the tool path is fine, other than it's cutting too much and chunks some edges and peaks. Maybe it's supposed to work that way and I need to adjust the step over?? Any help would be great
Attachment 394290

Please see the attached pic. The tool passes through the top right of the "R" at a.125" doc
I have tried lots of different approaches and anytime I have a border as part of the geometry I incur something similar. A simple v cut inside lettering works fine.

.converted bbcd o dxf and file is attached
Thanks Again-
Vince

[OldRustyIron]

I am having issues too version 30

[magicniner]

I've used V-Carve in V25 with the option to clear larger areas with an endmill first without issues, I just followed the procedure on the training DVDs

[The Engine Guy]

Hi Vince

Seems to work fine here, but hard to see on the old Verify here as my current Graphics Card doesn`t like it !!

Anyway, as you don`t say what tooling you are using I have gone for the default 0.25" End Mill and 0.25" 90 degree V tool, set the roughing to 0.125" DOC and also the V Tool to 0.125" DOC and it seems to work OK, only thing that might cause the V Tool to cut through lettering on the second DOC could be you clearance settings, if you have it set too low for example 0.2" then on the first cut it will miss the tops of the letters but not on the second, I set the clearances at 0.5" and it seems fine.

I have attached the file I did (V24 Build 546) which is pretty old so you should be able to open it, good luck with it, all I have at this time

Regards
Rob

[ironspyder]

Perhaps your safe z is set too low? Check your gaps in material setup?

[vpl]

Rob,
Thank you for taking your time and posting the file.
I'm using a 1" diameter 60* insert type vcarve tool and a .250 roughing bit.
I must be missing some basic skills. I have always set my rapid plane at .100" regardless of the type of work I'm doing, I have cut complex 3d mold faces with several doc's, both finish and roughing, never had an issue. I use .100" for my rapid plane on doing flat work such as sheet plastic or ply, several doc's, no issues.
I took a close look at the v carve tool path you made. I turned the path to red... It looks like the dot on the "i" is getting scalped by the v bit when it comes off of the perimeter cut. ???? It seems when the tool comes off of the perimeter is where the issue is.... any thoughts?
Thank you again!

[The Engine Guy]

Well spotted, it is on the other i dots as well and didn`t do the corners of the H right either, that`s what come with rushing My bad

I looked at it again and the only way I could find to get it to work was to change the V tool to a 30 degree (Included angle) one, works fine with that, set to any DOCs etc that works

Looks like you will need to go buy a 30 degree tool for that job unless anyone else has a better solution

All I have for now !! See attached file !

Regards
Rob

[vpl]

Well I believe I have solved the on going issues with bobcad-
http://https://release.vectric.com/products/vcarve/
When I purchased bobcad the salesman told me it was "mine for life", it is, only bobcad will no longer issue me a key if i have to reload it, so if my computer crashes I'm out of luck, if I want a new computer I'm out of luck.
I have been moving over to fusion 360, I would upgrade bobcad but I just can't justify it after the way they treated me during the sales process, worse than buying a used car. Plus I was mislead by the saleman's statement about my owing the program for life. Fusion doesn't v carve as far as I can tell and I have a lot of opportunity to do sign work- hence vetric-

Don't beat yourself up on this file, I don't think bobcad has the capacity to correctly execute this simple task-

[BurrMan]

Well spotted, it is on the other i dots as well and didn`t do the corners of the H right either, that`s what come with rushing My bad

I looked at it again and the only way I could find to get it to work was to change the V tool to a 30 degree (Included angle) one, works fine with that, set to any DOCs etc that works

Looks like you will need to go buy a 30 degree tool for that job unless anyone else has a better solution

All I have for now !! See attached file !

Regards
Rob

Looks to me like the letters are actually above Zero, and he has the top of part set at Zero!!!

So, "Scalping letter, yeah!"

But that's Ok now. He's moving to "Fusion"!

[BurrMan]

Yup.... Pretty much perfect!

[The Engine Guy]

Hi Burr

It is still doing those three moves here across from the edge to the i dots even with the geometry moved to Z zero, the only thing I could get to work was the change in cutter angle
BTW Fusion sort of reminds me of those dark BC V22 days when every "fix" broke something else, fun days those were

@VPL
But Hey Ho if a move to another software solves all your issues then that`s the way to go, good luck especially if you are going down the Fusion 360 route, not the best IMHO if you want to actually machine stuff

Regards
Rob

[vpl]

Looks to me like the letters are actually above Zero, and he has the top of part set at Zero!!!

Well thanks... I didn't translate the text after making it. I ASSUMED it was as zero. I moved it to zero and the tool path cleaned right up. Thanks!!! Very much appreciated !!

[vpl]

Burrman,
Seem as though I can get a clean cut. I attached a file and I must be still setting something up wrong-
The pocket depth is set at .250 and doc for roughing and v tool are set at .125 the v tool's doc is .250 on some of the letters and it takes 2 passes on others at a doc of .125???
The roughing tool path behaves nicely....
What gives? Thanks

[BurrMan]

With VCarve, the "V tool" is the finishing pass and strategy. So using an endmill to "rough" the material DEEPER than the finish pass, will not produce a good result.

I don't know why you have set it up this way, but it would be an incorrect way to use the toolpath.

Maybe more discussion on what you are trying to achieve, and input from some of the other machinists on how to get that could go along way.

I just set the finish cut depth to the same depth as the rough, and got a perfect result.

Maybe you are trying to do a "Chamfer" type look on the letters with that "Half depth" finish pass?

Rob would be more equipped to look at the operation. How an endmill roughs vs. what the 60 degree would leave at NOT a full depth. More information on what you are expecting to achieve with the backwards rough and finish settings could lead to an answer for the setup. Like breaking things into 2 operations or changing a depth per the 60 degree bit geometry, etc....

Anyway.......

[vpl]

Burrman,
I was trying to get the v tool to take more than one pass. When I cut deep letters the sharp points/corners get knocked off. I was trying to cut less per pass by reducing the depth and taking more than one pass....
I'm guessing by your reply the v tool or finish pass will only cut at the pocket depth and you can't make partial depth passes? I have even tried to cut super slow. When roughed with a straight end mill the bottom of the letter is very lightly cut, the top almost gets a full cut of 22..5* when using a 45* v bit...Is there an other strategy all together?
Thanks

[BurrMan]

I dont think that v finish has a "stepdown" setting. Its just a "depth" and a stepover. I'll have to look. I dont really fire up 24 much anymore.

If thats the case, i would add operations. Get rid of more rough before the v.

It could look like "make a pocket excluding the letters to use the bigger endmill, then make a boundry for just the letters, and use a smaller endmill in the rough portion of the vcarve.

Can look a bit later...

[BurrMan]

In vcarve, i think the steps are controlled by the depth and the bit geometry, to get that "bubbled carved" look....

[The Engine Guy]

Eric

Sorry for the delay, I think Burr is right with the splitting it up idea, I made a simple pocket around the ouside of the letters and then I set the roughing endmill to do multiple passes for the lettering, what it seems to give are a number of much smaller steps to take off with the V tool, yes, you can do more than one depth with the V tool as well, that would be something you would have to experiment with on the material being used as I don`t have any way to determine whether it would actually cut better for you.

Anyway, for now have a look at the attached file for a very simplistic example of what I think Burr is advocating, it can be expanded on if need be, might be more like what you need

BTW I still can`t get it to work with a 60 degree V tool.

Regards
Rob

[jrmach]

This was done with V23
As you can see,multiple step downs can have an effect you might not seek
In this case,intentionally done to look like this