Vcarve with pocketing

[Davo]

Is there a tutorial somewhere for this feature in aspire?

For the life of me I cannot get it to remove all the material around tight corners in the letter - not sure if I'm going about it wrong

[Kyle Stapleton]

Post a picture.
When you do a vcarve with a clearing tool the corners will look like it has little raises in it do to the fact that it's trying to clear with a v bit.

[scottp55]

Possibly add a screen grab in 2d view in Node edit mode zoomed WAY in to the problem area?
Sometimes loops/overlaps particularly in script fonts can give funky results.

[Davo]

I will get one tonight after work

[Brady Watson]

There isn't any way to get it 100% clean....but you can get real close.

See attached example toolpaths. First one with 1.25" dia bit @ 1%. 2nd with .5" dia @ 1%. It's a 'math issue' because of the diameter.

Unzip. Should open in any version of VCP or Aspire after 2010. (PW 2.5)

Be sure to preview each toolpath and hover your mouse over the 'leftover' areas to see just how much material is left...0.005" was the largest I measured from the v-bit 'wind row peaks' left over from that 1% stepover with a pointy tool...

The same rules apply on a regular pocket...You cannot get a square inside corner. If you didn't trunc the vbit from going full depth (neg prism) then you'd have a square inside corner.

Also...Just as smaller dia v-bits impart smaller stepover 'wind rows', smaller diameter end mills/bits impart smaller corner radii. So you can clean up that little area with an inside profile or small pocket using a 1/16" dia bit and you'd have a nearly invisible .03125" radius.

-B

[Davo]

2.8" letters with a 90 degree v-bit and pocketing with 1/4" endmill

26127

[Brady Watson]

I would consider 2 things.

1) Create sharp outside corners.

2) Machine the letters by themselves, then glue onto background.

If (2) isn't possible, create a vector boundary to go between in the E & S and use a small end mill to pocket it out flat. A 1/16" would probably do it, but this adds time.

-B

[Davo]

side question

i like the vbit texture it does when carving out an area, but it seems to slice a line straight through the middle

26128

[Brady Watson]

It is roughing out...and the tip of the tool stays low. There isn't any way around this.

-B

[Davo]

Brady - option 1 - how do I tell vcarve to make sharp corners on the letters?

[Brady Watson]

Abandon the V-carve strategy and use a 2D profile strategy. Choose from the options tabs to create 3D inside/outside corners...Play around, read the help file in that section, you'll get it...but there is no way around the radius/end mill issue. The best you can do is cheat with a pocket at the base of the letters to clear it out.

My approach would be to do the letters by themselves and stick them on after...

-B

[Davo]

Do vbits leave cleaner edges running slower IPS or faster?

[Brady Watson]

Slower. I usually V-Carve at 1.2,0.7 for most things; Less if very small and intricate. You have a 3-axis move going on there and if you are too fast (which the tool probably won't do anyway) every little reverberation will be 'felt' at the end of the tool tip.

Try experimenting in the same material at different speeds. See what is most obvious to you when you look at the quality of cut. Observe what the tool is doing during corner sharpening moves and lay your hand (safely) on the YZ car to feel the real story at different v-carving speeds.

There is no better experience than to witness first hand what is going on...

-B

[Davo]

What rpm are you normally running around at that speed?

[Brady Watson]

13-18k depending on material. As long as you aren't getting burn marks...it's all good.

-B

[scottp55]

Davo,
Just thought I'd toss my 2cents in as my brother asked at 11am if I could make a sign for him for Xmas for Mom and thought of you.
First shot was .1" flat depth with a 90VBit at 10% stepover with a .125" clearance tool and I was getting results like you.
Then I swapped to 6% stepover with same bit and a .0625" clearance tool.
Then tried a .08" flat depth to give a little more separation and used my Onsrud 60degree engraving/.01"flat with a 20% stepover and the same .0625" clearance tool.
Granted it's a one of for Mom, but a lot less sanding for me.
Just thought I'd post as long as I'm still working on the file.
scott
Oh, font was only 1.6" high though.
Garamond straight out of the box with no kerning.

[Davo]

Awesome Scott thanks!

And thanks again for the info Brady!

[Hizsigns]

Post a picture.
When you do a vcarve with a clearing tool the corners will look like it has little raises in it do to the fact that it's trying to clear with a v bit.

You may be trying to cut letters too deep. Remember that you have to account for radius of tool....sometimes you can also set offset of tool radius 1/2 of Diameter of tool. Hope this helps....

[Davo]

What do y'all normally have the pass depth for vbits at?

[Brady Watson]

What material? What diameter and angle bit? Important questions...

You have to ask yourself how much volume of material will be evacuated in one pass and ask yourself if that seems reasonable. Drawing the bit cross section in 2D can help illustrate this.

-B

[Davo]

I mainly use a 90 degree 3/4" and a 1.5/2"? 120 & 140 degree

3/4" oak / birch and Mdf

Normally I'm taking off 0.1 because it sounds the least stressful when it digs in

[Brady Watson]

Normally I'm taking off 0.1 because it sounds the least stressful when it digs in

Very good. Listening to what the tool has to say trumps everything else.

-B