too many Z moves while vcarving

[dr_when]

Hi,

I was wondering why when I vcarve an oval (see attached) I get a jillion Z moves... like instead of carving the oval, it makes a large number of "dots" around the oval. Subsequent passes are normal carving moves. I realize that normally I would not vcarve this but just make a profile with a V-bit. But it took me by surprise and took a long time to machine!!!

Thanks!!!

Bob

[RoutnAbout]

Bob,
I didn't run this file on my shopbot.
But I opened it up in Vcarve Pro, and looks like you created the smaller oval, Then offset the outside oval.
When you use the offset, The curved or arc line created with the offset icon will have lots of nodes.
You might try creating 2 ovals and see if that makes a difference.

[dr_when]

Don,

Oh gee whiz... that's it. It does seem like I have heard of this on the forum. My bad!! I have to let that little fact sink in a little more so I don't get fooled again!!!!

Thanks!!!

Bob

[dr_when]

This had me thinking (0h no) and I have to ask: Why would an oval when offset and having so many nodes, cause so many Z moves but not other vectors and curves that have many nodes? Does every node mean a Z movement necessarily? Just curious as to why this oval/offset anomaly works the way it does.

Thanks,

Bob

[RoutnAbout]

Bob, I can't answer that, I was only making an observation that there was lots of nodes one a offset vector.
I recreated the offset oval, And it appears that between those nodes are straight lines. So this will account for the extra moves.

There also will be a new feature " Curves Fit to Vectors" which will reduce those nodes in one of the next releases.

[BrianM]

This had me thinking (0h no) and I have to ask: Why would an oval when offset and having so many nodes, cause so many Z moves but not other vectors and curves that have many nodes? Does every node mean a Z movement necessarily? Just curious as to why this oval/offset anomaly works the way it does.

Thanks,

Bob

The constant distant offset of an oval is not an exact oval. In VCarve Pro the oval is drawn using beziers anyway, and again the offset of a bezier is not necesarily another bezier. Therefore to offset a bezier it needs to be approximated by a series of straight lines within tolerance which are then offset, this is why the offset is in turn made up of a series of small strraight lines.

When VCarve Pro 5 is released, there is a command to refit smooth curves to any polyline which will allow the offset to be refited as beziers (or arcs) within a user specified tolerance.

I hope that makes some sort of sense

Brian

[lstovall]

I think there is something else going on. I just download the file and there are a gazillion Z moves in the file. I ran a tool path for my router and there are no Z moves except at the beginning and end. Perhaps you might try a different post processor or maybe your driver software is configured wrong or differently than what you actually need. There are a lot of X/Y moves because of the segmented outer oval but no Z moves.

[lstovall]

Here's the crv file if you need it.

[Andy]

It looks like the multiple Z moves only happens when you have a flat depth defined for your VCarve toolpath AND, the pass depth of the tool is defined at exactly the depth of the cut.

Your ovals are spaced .2 inches apart. Your 90 deg v-bit "pass depth" is .1 inches. The tip of the bit will cut exactly .1 inches deep when cutting between the two ovals. Since the outer oval is line segments, the tip probably carves slightly deeper right at the point where the node is, and slightly shallower in the middle of the line segment. It's cutting the part below .1 inches in a 2nd pass. (why it only does it when a flat depth is defined is baffling me)

You can make it do a 2nd tool pass without all the z moves by setting your tools pass depth to .09 Or you can change the pass depth to 0.101 so that it does the cut in a single pass. Or, you can make the outer oval by offsetting by either .201 inches, or .199 inches (both of which are so close to .2 that you couldn't tell with the naked eye.

Either way, it's not a bug in VCarve. It's behaving precisely as it's supposed to given the circumstances.

[lstovall]

Interesting Andy.

Actually if you are trying to V-Carve you don't need to set the flat depth on that particular file. The way you have it set, the flat depth is more than it would cut anyway.

[Andy]

He probably needs the flat depth for what's inside the oval.

He could also define two separate toolpaths. One without flat depth for the oval, and one with flat depth defined for the rest of the artwork.

[dr_when]

Brian: Thanks... I knew that the offset created a lot of smaller vectors but forgot. Something for me to pay attention to.

Marv: It's interesting that you see the "jillion" Z plunges but your PP or controller seems to filter them out when cutting if I read you right. How does the PP or controller know that those plunges are not supposed to be there? (sorry if this is a dumb question... it's early and I need more coffee!).

Andy: Your explanation seems to get at the heart of the matter on why Vcarve would generate all those Z plunges. I understand in this case, doing a V carve in this situation with the dimensions used is not the wisest move. Again, for what I was going for a profile cut with a v bit would have been fine.

Thanks to all for your responses. It all indicates I have to take a quick look at the nodes on my artwork before cutting and be more cautious with the tool settings.

Regards,

Bob

[lstovall]

Bob,

To clarify. When I make the tool path using the V-Carve function without setting a Flat Depth, there are no unnecessary Z moves. The V-Carve depth is -0.1. If I set the Flat Depth to the same as the depth that the V-Carve will cut (-0.1), there are no unnecessary Z moves. If I set the Flat Depth to more than what the V-Carve will cut I have many unnecessary Z moves. If I set the Flat Depth to -0.09, I get the extra Z moves. If I set it to -0.08 I do not get the extra Z moves. If you need the Flat Depth for the center of the oval, I would suggest what Andy said. Make two different tool paths. Using the same bit, you could combine them into one tool path when you save them. If you are just wanting to do a profile cut with a V-bit, select the profile button (set the depth of the profile cut from there) and forget about the V-carve using the flat depth.

[dr_when]

Thanks Marv... it all makes sense. Funny thing too that I was actually asking Vcarve to do something that made no sense. I asked for a Vcarve width of 0.2" (determined by the offset of the two ovals ) at a depth of 0.2" with a 90 degree bit. There is no way a 90 degree bit could make that vgroove those dimensions. See attached.

[lstovall]

Yea, shame on V-Carve, trying to abide by the laws of mathematics. Glad you got it figured out.