V carving

[bryan]

Have been asked to v carve a sheet of baltic birch plywood, with "many" words on it approx 1.5" tall, I have it drawn up and was doing the cut file when i saw the step down was set at 0.03 per pass, with a 30 inch per min cutting speed. Going to use a 60 degree v bit. I'm thinking I can bump up the stepdown along with bumping up the cut speed, but how much? I know there are a lot more knowledgeable v carvers out there any help would save several hours on this project. Thanks

[paco]

Hi Bryan!

Soft wood might machine different than hard wood but I carve hard wood (http://www.cooptel.qc.ca/~usinum/artdesign_2.jpg) with a 60 deg. V tool at 0.188" stepdown at 1.5"/sec. at 19 000 RPM (a fast RPM with a sharp V tool will be better in soft wood) without any problem... in fact, I get very clean part. I suggest to perform some testing first... and would suggest a finishing clean up pass at full depth to avoid having to clean thoses sharp details...

[cnc_works]

I'm assuming you are talking about 3d centerline carving of letters.

You should be able to cut this in one pass with no problem, Bryan. I've cut 5/8" deep in one pass, but I was a little nervous at hearing the router bog down a little, of course it was only a 2.25 HP router, not the PC 7518.

You should also be able to bump the cut speed considerably, to 60 or 80ipm, though ramping will be the limiting factor anyway, I suspect. To a great degree, quality of cut depends on how tight you have everything adjusted because there are a lot of starts and stops and changes in direction in V carving.

Be sure to use a sharp bit to start with. BB has pretty abrasive glues in it. I remember routing a lot of it before I had a CNC and you could see where the glue lines ate into the carbide after some use.

Donn

[gerald_d]

You need to hold that sheet of plywood down very flat.

Most fonts at 1.5" tall will be okay with a single pass. You need only to worry about fat fonts (With them you might even go right through the ply)

I agree with the speeds mentioned above

[bryan]

Thanks
Paco, Donn, and Gerald for info will be testing it out tonight after the day job.
This is why the Shopbot is so great...this forum
helps all the newbees become better...
Thanks Again
Bryan

[evan]

Slight change to thread but fits with heading.
I've been trying to put a customers logo (very small only 1.5"long x .25" high and its on a diagnal)on the parts I've been cutting for them but whenever I import the text into PartWizard it wants to toolpath around the letters. If I V-carve them it'll take over a minute and a half for each part, and I've got 500 to do for each run. I don't have the margin to spend 13 hours cutting them. I want to use a Vbit but just one cut per vector, if you get what I mean. Any ideas?

[paco]

Evan,

look like your looking for a "single line font"... you can use the V carve's toolpath vector to draw 'em with the polyline tool (enable the snap to object)... or look for this kind of font... I could help; I've drawn some... mail me if your interested...
But I'm not sure that you'll gain much time than from V carving 'em full depth (single pass)... This is #@!?$ small; you'll need a VERY pointy tool bit!?...

[Brady Watson]

Evan,
For text that small, I would use a single stroke font like Paco suggests. If it is a logo, then you will most likely have to centerline the text in CAD or PW. If the text is that small, it shouldn't take you more than 1/2 hr to get that centerline perfect.

Once you have the centerline, use an engraving bit or a 60 degree V-bit at a depth of .01", using Machine Along Vector strategy. I would start at that depth and see how the logo looks. If the material is up and down all over the sheet, it may be difficult to get a perfect engraving on all of the pieces...so be sure your table is dead flat and the material is really flat and secured well. Believe it or not, if the Z height is out .005" you'll see it in the engraving from piece to piece.

-Brady

[joe]

Two more cents.

To keep the splinters down, on the top surface, I would paint a couple of good coats of shellac or any paint that will make the sheering cleaner.

On this kind of work, any little flaw can require a new panel. I'd make sure the z is set correct. On V carving it's everyting. Do a nice long test run on material that is the same thickness. In order to get the speed you would allmost have to do a test run.

I just finished doing a short run V carv and it took me more time to get the Z set than to do the whole job.

Good luck. Let us know how you did.

Joe
www.normansignco.com

[gerald_d]

"I want to use a Vbit but just one cut per vector, if you get what I mean. Any ideas?"

This illustrates a basic issue with V-carving software - some programs cut once, others cut twice. Our VCarvZ cuts twice, and it adds many surplus vertical moves. Apparently PartsWizard also cuts twice. A few years back we did have a demo of a program that cut once only and that made a big difference (The name escapes me now - it is often mentioned here, had a management change about 3 years ago).

If we have to speed up our VCarvZ "double-cutting" files, we take the file in dxf form to AutoCad and either:
- laboriously zoom-in and delete surplus moves, or
- slightly less laboriously trace a new toolpath over the inefficient one.