Inlay Pocket Tool path

This forum is for general discussion regarding VCarve Pro
Post Reply
markbachman
Posts: 12
Joined: Thu Jan 05, 2017 2:57 am
Model of CNC Machine: X Carve

Inlay Pocket Tool path

Post by markbachman »

Why does V Carve create a tool path like shown below? There are multiple raise and plunge moves that do not remove any additional material after the pass around the perimeter. This happens at each depth pass and greatly increases the cut time. I see no option to optimize tool path.
CRV file attached, look at tool path Pocket Inlay 1
Path Image.PNG
Attachments
Butterfly Inlay.crv
(982.5 KiB) Downloaded 34 times

User avatar
scottp55
Vectric Wizard
Posts: 3681
Joined: Thu May 09, 2013 11:30 am
Model of CNC Machine: ShopbotDesktop 5.5"Z/spindle/VCP10
Location: Kennebunkport, Maine, US

Re: Inlay Pocket Tool path

Post by scottp55 »

Mark,
Not fully caffeinated yet, and there will be other opinions/methods, BUT :)
Ran into this a BUNCH years ago doing 3D Owls in kid's building blocks for gifts....I'd make a boundary vector for the Model, and it Offset cut BEAUTIFULLY until the last 1% of cut...
And then my machine started doing a "Sewing Machine" imitation that took half as long as the cut itself.
I fudged/fixed it by using Curve Fit Vectors (Bezier) and Offsetting Inwards by a hair (and cutting to Selected Vectors with appropriate tolerance), and was soon cutting them 40% faster.

So I tried your file, and changed the original Female with a .005" tolerance....a Little better.
CURVE FIT VECTORS .005 BEZIER.jpg
Then tried .05"tolerance which distorted the Butterfly too much, But cut Lifts WAY down.
CURVE FIT VECTORS .05 BEZIER.jpg
Somewhere in between those two tolerances(OR Node edit the Female?) should be a decent cut? THEN copy THAT to the mirror layer and mirror it.
Brain should start working after this second cup...and I'll go DARN...there's an easier way....but I'll post now anyways.
scott
scott

User avatar
TReischl
Vectric Wizard
Posts: 3536
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: Inlay Pocket Tool path

Post by TReischl »

What you are seeing is the software calculating that there is a bit of material left between the .25 dia tool and the .125 dia tool. So it removes it.

I rarely use that large clearance tool option when doing pockets.

There is a lot more control over what is happening by using a pocketing tool path without that option and then creating a separate profile tool path. For instance, you can leave whatever you would like for a finish cut on the sidewalls of the pocket. Another thing is that you will get a lot more options on the profile tool, like ramping the cut instead of stepping down.

Here is a pic of what that profile tool pass looks like when the large clearance tool option is not selected:
Capture.JPG
Yanno I get the idea that just clicking a checkbox and selecting a tool is really convenient, but it seems that convenience comes at the expense of having control over the toolpaths. And that seems to be what you are wanting, so give it a try.
"If you see a good fight, get in it." Dr. Vernon Jones

markbachman
Posts: 12
Joined: Thu Jan 05, 2017 2:57 am
Model of CNC Machine: X Carve

Re: Inlay Pocket Tool path

Post by markbachman »

Ok I understand that there may be bits of material between the outer detail pass and the clearance pass. But why cannot it just stepover inwards and remove the material.
How can I submit this to the support team?

markbachman
Posts: 12
Joined: Thu Jan 05, 2017 2:57 am
Model of CNC Machine: X Carve

Re: Inlay Pocket Tool path

Post by markbachman »

Ok I understand that there may be bits of material between the outer detail pass and the clearance pass. But why cannot it just stepover inwards and remove the material.
How can I submit this to the support team?

User avatar
highpockets
Vectric Wizard
Posts: 3117
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: Inlay Pocket Tool path

Post by highpockets »

John
Maker of Chips

User avatar
TReischl
Vectric Wizard
Posts: 3536
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: Inlay Pocket Tool path

Post by TReischl »

markbachman wrote:Ok I understand that there may be bits of material between the outer detail pass and the clearance pass.
But why cannot it just stepover inwards and remove the material.
How can I submit this to the support team?
Probably is a good idea to send it off to support. I think your issue is an indication of a bigger problem:
Capture.JPG
Notice that the tool path of the profiling tool has crossed over the vector in several places resulting in rounded corners rather than sharp ones.

Interestingly if the vector is cut using a regular profiling pass on the inside this does not occur. A definite anomaly.
"If you see a good fight, get in it." Dr. Vernon Jones

User avatar
scottp55
Vectric Wizard
Posts: 3681
Joined: Thu May 09, 2013 11:30 am
Model of CNC Machine: ShopbotDesktop 5.5"Z/spindle/VCP10
Location: Kennebunkport, Maine, US

Re: Inlay Pocket Tool path

Post by scottp55 »

Ted,
That seems to be the standard behaviour for the normal Inlay Toolpaths(taking radius of the bit into account for Male and Female for a perfect fit).
But then I just finished surfacing a ratty piece of Oak firewood with a knothole in it...so what do I know :D
scott

User avatar
Adrian
Vectric Archimage
Posts: 10433
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Inlay Pocket Tool path

Post by Adrian »

TReischl wrote:
Notice that the tool path of the profiling tool has crossed over the vector in several places resulting in rounded corners rather than sharp ones.

Interestingly if the vector is cut using a regular profiling pass on the inside this does not occur. A definite anomaly.
That's what it's supposed to do otherwise the inlay won't fit. A profile pass is a different animal as it doesn't need to worry about the shape of another part.

User avatar
TReischl
Vectric Wizard
Posts: 3536
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: Inlay Pocket Tool path

Post by TReischl »

Thanks guys, for some odd reason I thought he was using a standard pocketing routine with a clearance bit.

I quit using the inlay tool a long time ago.

So my bad.

That said, I would still use the pocket and profile tools to get more control of something like this, but hey, that is just me!
"If you see a good fight, get in it." Dr. Vernon Jones

Post Reply