VCarvePro question: "Let My Cutter Pass"

[kfitz]

Let's say I run a pocket toolpath and find that the cutter can't make it through a narrow area. Let's say I edit the nodes to open it up a little to allow tool clearance. Obviously I want to widen the vectors just enough for the cutter to pass through, and no more. Question: Is there any way to know from the program at what point the tool will fit through the opening? Or even better, is there a "Let My Cutter Pass" button that will adjust all vectors that are too close together? Or do I have to do a trial and error approach using the preview?

[Brady Watson]

Kevin,
There is no function that I am aware of that will modify vectors so that a certain cutter will fit thru. I've always found it helpful to create a circle the same diameter as your cutting tool (eg - 1/4") and then 'drive' that circle around to see where it fits, then node edit as necessary.

Another trick that *sometimes* works on simple designs is to play with offsetting the vectors in & out to see if that can easily open up things for you...the problem is that it opens up ALL the vectors and this can distort the design in ways that are less than desirable.

-B

[nschlee]

The ability to use multiple fill tools similair to Enroute would help. I asked them to put it on the wish list.

Neal

[Brady Watson]

Neal,
Are you talking about 'rest machining' ? ArtCAM Insignia & Pro will do this. You'd use your 1/4" tool and then tell it you want to use a 1/8" tool. Then it will ONLY toolpath where the 1/4" doesn't get.

-B

[knight_toolworks]

the circle is a good way. but even then it may not fit. I was doing these wedge shapes and I had to go .4 to get a .357 bit through.

[beacon14]

When nesting shapes in DesignCad I'll sometimes make an offset line from a shape, move the next shape until it touches the offset line, then delete the offset. That way I have exact control over the spacing

[nschlee]

Brady sounds like the same feature. I use it quite a bit in E3, it can save a fair amount of machining time on large filled areas. Mostly I use .5", .25", .125" & V Bit of choice, E3 creates all the toolpaths leaving very little if any cleanup. Just V carved a 3'x4' mahogany sign with lots of fill, I chose E3 over VCP4 for this job as it had this feature and VCP does not. IMO, VCP NEEDS this feature in it's tool box!

[jsfrost]

I use Brady's circle trick frequently to see what vector changes might give the right appearance. But sometimes, for me, the easy way is to draw a single vector line or two where you want the bit to pass, and run a separate machine along vector toolpath.

I agree with Neal, VCP needs to do area clear with multiple tools. VCP lacking this feature often has me returning to Insignia.

With the feature I would like the ability to manually cleanup the toolpath on screen, leaving the significant small bit area clears and eliminating small bit "pecks" that, in an artistic cut, add sanding, but do not add meaningful detail. As far as I know neither Artcam nor VCP presently allow selectively deleting toolpath segments.

[tony_mac]

Hi Kevin,

There is a 'trick' that makes it possible to use the Flat Bottom VCarving Toolpath strategy to calculate 2 toolpaths - an End Mill for removing the stock material followed by a smaller cutter that only machines regions where the larger first end mill does not fit. I will email the details to you.

For reference - VCarve Pro 4.5 is about to be released and this includes a new option for previewing toolpaths in the 2D window as a solid colour fill. This functionality makes it very clear to see where the selected cutter can and cannot fit. The design can then be edited manually using the node editing tools to open up regions allowing the tool to fit if required, as Jim suggested.

More details about VCarve Pro 4.5 will be emailed to customers and posted on the Forums in the next few days.

Tony

[kfitz]

That would be brilliant Tony; thanks!

[waynelocke]

Tony,

Can you post the trick somewhere for wider dissemination?

[jimmya]

I also would like to know the trick too. I have a job right now that need to use 2 flat bit for area clearing.

Jimmy

[mziegler]

By using the offset tool you can easy see if the tool will reach all areas to be pocket. By offsetting inward by half of the tool diameter will show the toolpath that Vcarve will calculate. Mark