First CNC Project

An area to upload images of pieces cut using VCarve Pro
hershey932000
Vectric Apprentice
Posts: 9
Joined: Mon Oct 21, 2013 6:25 pm
Model of CNC Machine: G0704

First CNC Project

Post by hershey932000 »

Hello all! I have just begun this creative voyage into CNC and I am loving it. I have had a few dramatic moments in the garage spilling tears onto my machine (broken bits/crappy clamping etc.) but I'm sure at some point in the learning curve tears become replaced by restrained frustration. As a first project I decided to make this gift/promotion plaque for a family member. My question is, for those who have been there/done that with small text engraving, what kind of bits are you using? I used a 15 degree profiler with a .010" tip, running at 2250rpm, pass depth .001, 5% stepover, 6 IPM and a plunge of 3 for text that measured .22 inches. It took forever, as you can likely tell from these numbers. What kind of bits do you recommend for this kind of text to minimize time while not sacrificing quality or depth? Also, any other general recommendations to improve upon this kind of project? I'd like to make more for promotions in the unit and I want to the best job I can for their special day. Thanks for your time -- Aubry
20140226_045557.jpg

glenninvb
Vectric Wizard
Posts: 1129
Joined: Thu Jul 18, 2013 4:58 pm
Model of CNC Machine: homebuild / VCP 8.0

Re: First CNC Project

Post by glenninvb »

Hi Aubry,

Being you haven't gotten any replies yet, I'll give it a go.

Trying to machine wood with a GO709 is going to have limitations with a max spindle speed of 4300 rpm but I guess it can be done. Most woodworking bits are designed to turn 8000-25000 rpm. I would try to use 3-4 flute mills for best finish at those rpms

To answer your main question, A small .005 tip profiler is good for very small or shallow engraving (I guess it did take a while!)

A 1/2"60 degree V-bit (using V-carve toolpaths) would cut most of the text on your plaque nicely. Use max rpm's and try 20-30 ipm (just guessing)
The pocketed SFPD at the top could be cut with the same bit by specifying a flat depth of say .030 or you could use a end mill, looks like a 1/8" would fit, that's what the preview is for.

Try to use the largest tool that will fit the job. The only time I use a .005 tip v-tool is for engraving cast acrylic or metal and at a depth of .005-.010 and 15-20000 rpm using the quick engrave function

Just my opinion, and I'm novice, sure someone else will chime in

Nice job on the Plaque

glenninvb
Vectric Wizard
Posts: 1129
Joined: Thu Jul 18, 2013 4:58 pm
Model of CNC Machine: homebuild / VCP 8.0

Re: First CNC Project

Post by glenninvb »

Aubry,

Just to see what it would look like and I think you will be amazed at the time difference!
select your text and select 1/2" 60 V-bit, select the V-carve tool-path and then preview

Don't forget to increase the pass depth

And sorry, meant GO704, did you convert it yourself?

Glenn

hershey932000
Vectric Apprentice
Posts: 9
Joined: Mon Oct 21, 2013 6:25 pm
Model of CNC Machine: G0704

Re: First CNC Project

Post by hershey932000 »

Glenn, thanks for the reply! I plugged the 60 degree, 1/2" bit into V-carve with your suggested IPM and I have to say, 6 minutes sounds like a dream compared to what I was suffering through before. The preview text looks a little bit ragged, but it got better if I increased the flat depth to .015. How smooth should the preview text appear before you turn the machine on? I have been relying on V-carve pro previews to look perfect before I go to the machine, which is why I am ending up with tiny bits and very long wait times. Have you found the preview to be an accurate indicator of how it turns out? If so, do you think this text would be acceptable?
preview.jpg
I didn't do the conversion myself, I bought it turn-key from Midwest Machine Works. My long term goals are to work with metals and I wanted something heavy, rigid and durable. I'm very happy with it, it has been a good machine to learn on and grow into. I realize I'm limited by RPM's and table travel on my machine so I found a shop in Austin called Make+Shift and got certified to use their ShopBot, so in the future I will probably take my woodworking projects up there.

User avatar
FixitMike
Vectric Wizard
Posts: 1744
Joined: Sun Apr 17, 2011 5:21 am
Model of CNC Machine: Shark Pro Plus (retired)
Location: Burien, WA USA

Re: First CNC Project

Post by FixitMike »

For lettering, I put a coat of the finish varnish (thinned if it is oil base) or sealer on before I fill the letters with their contrasting color. I do a quick wipe before it dries, and then sand the rest of what has gotten on the top surface off after it dries. If you are using an open grain wood like red oak, a coat of wood filler before you start can help.

For a simple inlay, fill the VCarved letters with Plastic Wood filler and sand flat after it hardens.

For a real mind blowing wood lettering inlay, look up the VCarve inlay method. (Mind blowing in both appearance and figuring out how to do it.)
Good judgement comes from experience.
Experience comes from bad judgement.

glenninvb
Vectric Wizard
Posts: 1129
Joined: Thu Jul 18, 2013 4:58 pm
Model of CNC Machine: homebuild / VCP 8.0

Re: First CNC Project

Post by glenninvb »

Aubry,

Don't specify a flat depth unless you need a flat pocket, or unless your engraving a single line font (then the quick engrave can be used)
If you specify a flat depth the point of the cutter will leave lines as it steps over (sharp point)

The width of the text vectors will determine the carving depth with a V-bit, the 60 deg. works best for small text

For pocketing use a center cutting endmill that will fit inside the vectors or use a V-tool with a flat point (as large as possible) and only the edges of the pocket will be angled 1/2 included bit angle.

This is cut with 1/2" 60 deg. V-bit with Pass depth set .050 The 1" text cut depth is .139
The preview is what you get!!!!

Glenn
Attachments
Capture.JPG test.JPG

glenninvb
Vectric Wizard
Posts: 1129
Joined: Thu Jul 18, 2013 4:58 pm
Model of CNC Machine: homebuild / VCP 8.0

Re: First CNC Project

Post by glenninvb »

Forgot to mention, if you convert the text to curves (4 rows down 4 over in Vector tools, object to curves) you will get the best results
It's a node thing, but your doing good
I learn something here about every day, if I could only retain it!

Watching the tutorials is very valuable, and get some scrap and test, then put it all together and make something........ :mrgreen:

br1
Vectric Apprentice
Posts: 53
Joined: Wed Feb 25, 2009 12:19 pm

Re: First CNC Project

Post by br1 »

I think you did very well "As a first project". Nice

tmerrill
Vectric Archimage
Posts: 4797
Joined: Thu May 18, 2006 3:24 pm
Model of CNC Machine: ShopBot
Location: North Carolina

Re: First CNC Project

Post by tmerrill »

Forgot to mention, if you convert the text to curves (4 rows down 4 over in Vector tools, object to curves) you will get the best results
It's a node thing
Glenn,
Are you saying that simply converting text to curves before v-carving results in better results?

If so, give this a try:

Take a single letter of text and create a v-carve toolpath for it. Save it as a cut file.

Now convert that letter to curves and create a v-carve toolpath for it using the same bit and setup parameters. Save it as a second cut file.

If you then compare the cut files I think you will find them exactly the same, which means the letter shape is being toolpathed the same irregardless of whether it is text or curves.

Text is simply vectors grouped with a unique attribute. As text, you can easily re-open it and make changes using the Draw Text tool. Converting it to curves removes this text attribute and while you now have more control over different aspects of it, you have lost the ability to edit it as text. In my opinion, one should not convert text to curves unless there is a compelling reason to do so.

Tim

glenninvb
Vectric Wizard
Posts: 1129
Joined: Thu Jul 18, 2013 4:58 pm
Model of CNC Machine: homebuild / VCP 8.0

Re: First CNC Project

Post by glenninvb »

Tim,

I agree it does hurt your ability to edit, I was told (here) at some point converting text to curves removes un-needed nodes and will smooth point to point tool-path calculations?
But I just checked and the same nodes exist both ways?

I'd like to hear more about this subject.

And anytime I give bad advice, please step in, no offence taken,(we may not always agree on every subject) Like I said I learn something here every day and appreciate it.

Thanks,
Glenn

User avatar
Mike-S
Vectric Wizard
Posts: 1123
Joined: Mon Jun 13, 2011 6:45 am
Model of CNC Machine: Joe's Hybrid 4x4 (but 3x3)
Location: Hayesville, NC

Re: First CNC Project

Post by Mike-S »

Concerning smooth cuts, consider this "S"

The original text was converted to curves,
then the vectors were off-set (note all the nodes),
then "Fit curves to selected vectors" (Bezier) got rid of all the little jerky cuts.
Attachments
FitCurves.jpg

tmerrill
Vectric Archimage
Posts: 4797
Joined: Thu May 18, 2006 3:24 pm
Model of CNC Machine: ShopBot
Location: North Carolina

Re: First CNC Project

Post by tmerrill »

I'm not sure what point you are trying to make Mike. You do a lot of steps to go from Bezier curves with 31 nodes to Bezier curves with 27 nodes, a difference of only 4 nodes.

On my machine, Bezier curves are cut as straight line moves but I have never had any issue getting poor results with v-carved toolpaths. If I were to follow your steps, with the intent to cut it on my machine, I would simply convert to curves and then convert the Beziers to arcs as my machine cuts arcs with arc commands - no need to offset.

Tim

User avatar
Mike-S
Vectric Wizard
Posts: 1123
Joined: Mon Jun 13, 2011 6:45 am
Model of CNC Machine: Joe's Hybrid 4x4 (but 3x3)
Location: Hayesville, NC

Re: First CNC Project

Post by Mike-S »

No, I didn't mean that to be a work flow. Only that after an "Offset" that produces many nodes, there is a way to smooth out the curve again. Sorry to muddy the discussion. :oops:

tmerrill
Vectric Archimage
Posts: 4797
Joined: Thu May 18, 2006 3:24 pm
Model of CNC Machine: ShopBot
Location: North Carolina

Re: First CNC Project

Post by tmerrill »

Thanks Mike, now I understand.

Tim

glenninvb
Vectric Wizard
Posts: 1129
Joined: Thu Jul 18, 2013 4:58 pm
Model of CNC Machine: homebuild / VCP 8.0

Re: First CNC Project

Post by glenninvb »

First,
Sorry to the OP for hijacking your thread.

Tim, Mike,

If I understand correctly, which is debatable, the only time you should convert text to curves is to be able to node edit ?
Any other reason?

Post Reply