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 (http://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.

[srwtlc]

Gerald,

That would probably be Rams3D (http://www.rams3d.com/ddex.htm) that you're thinking of. A demo should be available yet.

[gerald_d]

Yes, it was Rams - thanks Scott.

[btk]

I have noticed that Partwizard creates "double" passes even when they are not necessary (i.e. single pass in other software for the same dxf).
Additionally, Partwizard only shows one pass on the screen, however if you look at the file (or machine in action) there are additional cleanup passes.
Image on left shows Partwizzard Screenshot and Second image shows "hidden" passes.

4916
4917

[Brady Watson]

I'm pretty sure that PW does the 'extra' passes as a measure to clean-up the carving. I *believe* that it does a final climb-cut pass, as you would on any inside cut, to clean up the fuzzies.

-Brady

[paco]

BTK,

Thoses "hidden" pass are actually what I would call roughting pass; when a tool is set to a stepdown lower than the actual total depth of the V carving... in other words, if one setup the stepdown of a tool greater than the total depth of the V carving, it will perform the carving without thoses "hidden"/roughting pass... but thoses roughting are usefull on larde/deep carving...
"Clean up pass" too are VERY usefull; one would hate to have to hand clean thoses grooves... I've found that the machine will clean up V carving about 50-75% faster than me!...

[gerald_d]

The one pass system of RAMS was very good. We never do clean-up passes with any other cutter, and don't like the way that our VCarvZ forces us into a second pass. If the 2-pass programs want to be efficient they should give you a choice of one, or two, passes - but I think that their center-finding process forces them to cut "twice". I believe that these 2-pass programs actually go once around the perimeter of the letter, calculating offset and depth - this makes it look like two passes.

[evan]

Thank You Everyone for all the imput.
Paco & Brady -I'll try to find the font in "single line" or centerline it in AutoCad, but first I'll check the step down on the Bit. Even if I can only reduce the time to a minute or so a part it'll be worth it.
By the way it's only 8:40 out here on the West Coast. Sun is shining.

[gerald_d]

Over here it is 6.51pm and the sun has just set. Good to see that the server clock (in the date/time line above) is back in synch.

[Brady Watson]

Evan,
If you are using PW to 'v-carve' then you will be forced to do a Machine Along Vector, because once you change any of the 10 v-carvable fonts, it tells you that it's a no-go.

This is why I suggested centerlining the logo, and using a MAV strategy at a single depth that you set after experimenting with the best look in a piece of scrap. It will just engrave the centerline, and will not sharpen the corners. On letters that small, it shouldn't make a difference...and this will speed up the process tremendously.

-Brady

[evan]

Had to go out to a site so I just got back about half an hour ago. I centerlined, used a 60V-bit & MAVed it all in PW. It only takes 25 secounds to carve an induvidual logo now YeeHa!! Usually I reinvent the wheel(I get a perverse pleasure out of figuring it out myself) but this time I decided it would be a lot faster just to ask. Thanks again everyone.
Happy Friday!

EMC2

[btk]

Paco,

In this instance, a roughing pass is not necessary to clear the material as the diamter of the tool (3/4" 60 deg. V-Groove) is sufficient enough to clear the groove in one pass and I set my stepdown enough to reach the centerline.

--------------------------
Brady,

The "hidden" passes are actually done before the centerline pass (see attached image showing order of passes). The centerline passes are the final passes done.

-------------------------------------
I actually have no problem with Cleanup and/or Roughing passes, however I was just pointing out that they are not shown in Part Wizard.

As Gerald mentioned, I think it would be advantageous to be given the option (based on the material being cut and required finish) to forgo the rough passes. However in all instances, I would like to see them on Part Wizard.



4918

[bryan]

Well it took all of sat and sunday to do all of the v carving on 330 plaques, but if it wasn't for some friendly advice on cutting speeds and depth I just might be cutting till next weekend.
have attached a photo of the bot cutting out the last sheet of plaques.
4919
4920

[3d_danny]

Bryan,

Do you have a larger picture? I would really like to see a closeup of the plaques, if you have one.

Dan

[bryan]

Dan send me a email crismas@columbus-ks.com (mailto:crismas@columbus-ks.com) and I'll send you back some bigger photo's after I get home tonight