Toolpath optimization

This forum is for general discussion about Aspire
randyr
Posts: 45
Joined: Thu Jan 23, 2014 4:36 am
Model of CNC Machine: Speedline (Carl Bruce)
Location: Boring, OR USA
Contact:

Toolpath optimization

Post by randyr »

I have a simple job...just a bunch of wavy lines one right above the other. The start point for each line is on the left, going to the right. When I generate an "on" toolpath, the cut ALWAYS starts at the start point of each line. It doesn't matter if the "use start points (don't optimize) is checked or not...the toolpath is identical. This results in a G0 move back to the start for each line, when it should just go up a fraction to the next line. It doesn't matter if it's climb or conventional (which shouldn't matter for an "on" cut anyway. For a large number of long lines, this is a LOT of wasted time.

Is there something I'm doing wrong. or is this a bug (i.e. optimization not working right)...or simply the way it works. I could, and have, manually changed the start points of every other line and then it works the way it should, but that's a pain.

I've included a sample file (straight lines...the wavy line one was too big..)

Thanks,

randy
Attachments
straight_lines.crv3d
(53.5 KiB) Downloaded 129 times

User avatar
IslaWW
Vectric Wizard
Posts: 1380
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: FabMaster ATC-40 Bridgemill
Location: Marquette, MI, USA

Re: Toolpath optimization

Post by IslaWW »

Randy...
All of the start points for every vector shown in your example are on the same end (left). This means the machining MUST start on that end.
With the file open, enter node edit mode [N] key or icon, and place a start point on the right end of every other vector. That will allow the toolpaths to be generated in the way you want.

I did a few... see below
Attachments
Alternate.JPG
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

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

Re: Toolpath optimization

Post by glenninvb »

If your using linear array to duplicate the lines, you can just draw two lines with desired spacing and change start point on one line before using array tool.

randyr
Posts: 45
Joined: Thu Jan 23, 2014 4:36 am
Model of CNC Machine: Speedline (Carl Bruce)
Location: Boring, OR USA
Contact:

Re: Toolpath optimization

Post by randyr »

Thanks for the answers. Yes...I KNOW the start points are all on the left (I mentioned that post). Yes..I KNOW that I can manually change every other one (also mentioned). My working file has hundreds or lines, all slightly different...imported, not generated by Aspire (modified sine waves, all with a slightly different start on the wave...guilloche patterns). Not generated by Aspire...imported. With hundreds of lines, manually changing every one is a bit of a hassle.

You'll notice that on the "profile" toolpath page there is a checkbox that says to use the start points. That, to me, implies that when that checkbox is not checked, it doesn't always start at the start point. If it did, thenwhat's the purpose of that "use vector start point" checkbox?

So...my question still stands...is there something I can do for it generate better toolpaths....with those start points unaltered. Or is that just the way it works. And when does that "use start points" checkbox come into play?


thanks.

rr

User avatar
Adrian
Vectric Archimage
Posts: 13077
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Toolpath optimization

Post by Adrian »

There are various strategies available under the Order tab (make sure you have Advanced Toolpath Options checked). One of those might give you a better result but I don't think anything will match doing it by hand.

randyr
Posts: 45
Joined: Thu Jan 23, 2014 4:36 am
Model of CNC Machine: Speedline (Carl Bruce)
Location: Boring, OR USA
Contact:

Re: Toolpath optimization

Post by randyr »

Ah...the "order tab". Thanks. I didn't see that. I do see where there is a "shortest path" option that wasn't checked. So...I checked it, and unchecked all the others...and....

...no change. It still uses the start points. No matter what is checked, the same path is generated...obviously there is something that is causing it to not do any optimization. I'll play around more and try to find some combination of options that will actually cause whatever optimization there is to work...although maybe it's time for a support call.

Thanks again for your help....

rr

randyr
Posts: 45
Joined: Thu Jan 23, 2014 4:36 am
Model of CNC Machine: Speedline (Carl Bruce)
Location: Boring, OR USA
Contact:

Re: Toolpath optimization

Post by randyr »

So...not to belabor the point, but, just for grins, I rotated all the lines so all the start points are on the right (so the line goes right to left) , then checked the "use left to right" box on the "order tab"...and...no difference. It still uses the start points, and goes right to left. There doesn't seem to be any way for it to not use the start points.

Now...I'm not complaining. I very much like this program...I'm just trying figure out what works and what doesn't. There is clearly either a problem with their optimization code (why have those nice options if they don't do anything)...or with my understanding of how to use them.

rr

User avatar
BrianM
Vectric Staff
Posts: 1962
Joined: Mon May 16, 2005 10:15 am
Model of CNC Machine: A few ...
Location: Alcester U.K
Contact:

Re: Toolpath optimization

Post by BrianM »

Hi Randy,

The use start points option is for machining closed vectors. For closed vectors the software when it has finished machining one profile will by default reorder the closed contour to move to the nearest node, setting this option will prevent this behavior.

Regards

Brian

User avatar
TReischl
Vectric Wizard
Posts: 4294
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: Toolpath optimization

Post by TReischl »

The issue you describe is actually a difficult software problem to solve, if there is a solution.

I wrote commercial CAD/CAM software for over 20 years and had the same issue. At first blush it seems like a simple problem, but after digging into it, it is way more complex than first appearances.

Yes, the software could look at a path of vectors, check the endpoints and decide if the opposite end is closer and then reorder the sequence. No big deal. But not all non closed tool paths line up down one side of a drawing, remember, you are dealing with one example, there are infinite possibilities. So, what happens on other examples is that the tool path may creep to the wrong side no matter what.

What you are asking about is actually a version of what is known as the TSP (traveling salesman problem) in software develop. With a little research you will discover that it is extremely time intensive problem to solve. Programs you see that develop shortest route scenarios (typically on line map type programs) rely on the user to state the order in which locations will be visited. However, for a simple trip they will pick the shortest route. They are fast because they use parallel processing techniques (lots of computers working on a portion of the problem at the same time).

Then there is the small issue of those who want to cause the machine to cut in the same direction for every cut due to grain concerns or they could be machining an edge and they want all edges to be cut with the same tool direction. One would have to add another option.

The real skill of software development is not how many options can a company put in the software in an attempt to satisfy every possible demand, but rather how to keep the user interface uncluttered and not bloated to the point that it becomes cumbersome. In other words, sometimes the option does not have the demand to outweigh the negatives of not providing the "feature".

I have operated programs that have endless lists of options. Remembering which options to turn on/off and which menu they are located in becomes very tedious.

Is manually moving the start points in your example tedious? You betchya. But then it is not something that occurs all that often for the majority of users.

Cheer up, it could be a lot worse, you could fall into the "way back" machine and have to program all those curves manually. Calculating each and every curve, start point, end point, I and J values. Then have to type them in and hope you do not make a typo. Ugly business! I used to do that for a turret punch. 1200+ hits to cut around a window opening in cab for a piece of construction equipment with angled windows and radiused corners.

Just trying to give you some perspective with this comment. It is not that the Vectric Team is not smart enough, or lazy. It is more the nature of the problem and will providing a solution appeal to the most users without bloating the software.
"If you see a good fight, get in it." Dr. Vernon Jones

randyr
Posts: 45
Joined: Thu Jan 23, 2014 4:36 am
Model of CNC Machine: Speedline (Carl Bruce)
Location: Boring, OR USA
Contact:

Re: Toolpath optimization

Post by randyr »

Thanks for the explanations.

rr

User avatar
TReischl
Vectric Wizard
Posts: 4294
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: Toolpath optimization

Post by TReischl »

Curious, Randy? I see you have a "home built" machine. Me too.

My first one was a screw type machine. The rapids were slooooowwwww, like 80 IPM, drove me nuts. I finally built a rack and pinion machine so now I can easily rapid at over 400 IPM. Makes things like you are doing more tolerable. The lasers I worked on just before retiring rapided at about 2400 IPM. Incredible to see that much mass move that fast!
"If you see a good fight, get in it." Dr. Vernon Jones

randyr
Posts: 45
Joined: Thu Jan 23, 2014 4:36 am
Model of CNC Machine: Speedline (Carl Bruce)
Location: Boring, OR USA
Contact:

Re: Toolpath optimization

Post by randyr »

Well...maybe I should update my profile. My first machine was homebuilt, a small fixed gantry, movable table machine. Then I upgraded to a commercial machine, built by Carl Bruce up in Seattle....

http://cncbuilder.net/

Carl builds them in his garage shop...so...I suppose it's still a homebuilt.

rr

User avatar
IslaWW
Vectric Wizard
Posts: 1380
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: FabMaster ATC-40 Bridgemill
Location: Marquette, MI, USA

Re: Toolpath optimization

Post by IslaWW »

Randy...
If you read between the lines, and I don't mean to put words in Brian's mouth, there is a "use start point" option for closed vector shapes that can "force" machining to start at a given node. If you read into that, there is NOT an option to optimize in that way for open vectors. Machining operations will always start on the start point of open vectors. There is the caveat of climb/ conventional direction that is enforced.

In the long run, this allows complete control over the machining direction, but, as in your example, doesn't present the most efficient appearing toolpath when using numerous "bulk generated" open vectors. You need to choose which takes longer, node edit of the required start point changes or using a full length rapid between vectors.
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

ger21
Vectric Wizard
Posts: 1592
Joined: Sun Sep 16, 2007 2:59 pm
Model of CNC Machine: Custom DIY
Location: Lake St Clair, MI, USA
Contact:

Re: Toolpath optimization

Post by ger21 »

Is there any way to change the start point of the vectors when they are created?

I'm a firm believer that all vectors should be drawn in the correct direction, with correct start points, before the CAM ever sees them.
Only takes a short time to do this up front, and makes things much easier at the CAM stage.

And this allow you to have far more control over the resulting toolpaths.
Gerry - http://www.thecncwoodworker.com

User avatar
TReischl
Vectric Wizard
Posts: 4294
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: Toolpath optimization

Post by TReischl »

ger21 wrote:Is there any way to change the start point of the vectors when they are created?

I'm a firm believer that all vectors should be drawn in the correct direction, with correct start points, before the CAM ever sees them.
Only takes a short time to do this up front, and makes things much easier at the CAM stage.

And this allow you to have far more control over the resulting toolpaths.
Maybe a short time with really simple parts. I don't know about you, but if I want to design something like a rectangle that intersects with a circle I use the weld tool. Drawing five separate lines and an arc individually would be ridiculous.

And then, there is the little problem of the designer having to know what kind of machine was going to do the work and all the stuff a good programmer knows about tooling, setup, clamping, etc. Nah.
"If you see a good fight, get in it." Dr. Vernon Jones

Post Reply