Tool path optimization

This section is for useful tips and tricks for Aspire
Post Reply
SawdustandSmoke
Vectric Apprentice
Posts: 57
Joined: Thu May 02, 2013 1:46 am
Model of CNC Machine: home made

Tool path optimization

Post by SawdustandSmoke »

Hello! is there a way to force aspire to finish a 3d finish cut before moving on to the next cut without making them all individual?

The problem I'm having is that it will do half a carving and then start on the second, by the time it gets back to the first one the wood has moved slightly which leaves a faint line I have to sand out.

PaulRowntree
Vectric Wizard
Posts: 1687
Joined: Sun Oct 24, 2010 7:28 pm
Model of CNC Machine: homebuilt 4'x2' (Mach3+G540)
Location: Guelph, Ontario
Contact:

Re: Tool path optimization

Post by PaulRowntree »

I'm not sure how you mean, it should finish one toolpath before moving on to the next.
On a different note, you should be able to secure the material better.
Paul Rowntree
WarpDriver, StandingWave, Topo and gadgets available at PaulRowntree.weebly.com

User avatar
zeeway
Vectric Wizard
Posts: 3157
Joined: Thu Feb 11, 2010 9:24 pm
Model of CNC Machine: Self-built
Location: SC, USA

Re: Tool path optimization

Post by zeeway »

I just did a 3d project (cathedral window model) where I very cleverly cut out some areas and then omitted those in the 3d toolpath. That had the toolpath stopping and starting all over the place. I finally stopped it, and just redid the 3d toolpath to cover the entire model. It started from one end and went to the other without stopping. So...sometimes what you have done beforehand will affect the toolpath behavior.

Angie

SawdustandSmoke
Vectric Apprentice
Posts: 57
Joined: Thu May 02, 2013 1:46 am
Model of CNC Machine: home made

Re: Tool path optimization

Post by SawdustandSmoke »

What I am doing is copying and pasting the models and there vectors over and over again when I have a large amount of material. When I go to to recalculate the tool path's I shift click the vectors and hit calculate on each tool path. Problem is it cuts a portion of the model then goes on to the next then comes back and finishes them. Maybe I am not selecting them right ?

User avatar
TReischl
Vectric Wizard
Posts: 3362
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: Tool path optimization

Post by TReischl »

It sounds like you have vectors around each model? Then you "shift click" on the vectors, which makes it sound like you are selecting all the vectors and calculating a tool path. Doing that allows the software to look at all the models and make decisions about when to move to another model.

Try selecting one vector around one model and calculating the toolpath. Then move on to the next one.

Of course, you should be able to calculate all the roughing paths in one go because the moving around will have no effect on the final finish passes.

SawdustandSmoke
Vectric Apprentice
Posts: 57
Joined: Thu May 02, 2013 1:46 am
Model of CNC Machine: home made

Re: Tool path optimization

Post by SawdustandSmoke »

Right now that is what I am doing one vector at a time, and this is useable but I would like to not have 12+ finish toolpaths in my tool path window if there is some way around it. I know profile cuts you have some control over the order but I'm not sure if 3d does.

tmerrill
Vectric Archimage
Posts: 4797
Joined: Thu May 18, 2006 3:24 pm
Model of CNC Machine: ShopBot
Location: North Carolina

Re: Tool path optimization

Post by tmerrill »

Here is a trick I use frequently as I always raster with the grain, and I think this is the direction Angie was pointing you towards in his post above.

As with everything, there are trade-offs. In this case there is an increase in setup time, increase in machining time and it may not work with your overall design. But, if it does work, the trade-offs are minor for me as I do not like to spend time sanding when it can be avoided.

Basically, you need to create a machining boundary that does not create regions that need to be cut individually. A good example is the Anchor included in the Aspire clipart. If you look at the first picture you will see that by simply using a vector that hugs the shape there are numerous retracts and plunges (green vertical lines). These create the issue you are seeing.

Now take that vector and use the Offset Tool to move it out a large amount and then move it back in a slightly less amount. In the second picture I offset the vector boundary created in Aspire by 4" and then offset the new vector back inwards by 3.9" to create the new machining boundary.

Use this new vector to recalculate your toolpaths and as you can see in the third and fourth pictures there are no retracts during the cut - the raster starts at the bottom and cuts continuously until it reaches the top where it retracts.

In this example you could even take the time to node edit the new boundary vector by bringing the sides farther in, just don't create a shape where the bit can't flow continuously from one edge to the other. As a different approach, shapes like the anchor can also be done easily with a series of rectangles drawn around it and then welded to form one shape. Once you understand the concept looking at a model's shape should lead you to the best way to create the new machining boundary.

Once you have the vector where you want it, position them as a matched pair and set your final toolpaths up. Each finish toolpath should start and finish a model before moving on.

Tim
Attachments
Retracts with close boundary.jpg
Offset vectors.jpg
new finish toolpath.JPG
finish toolpath no retracts.jpg

Post Reply