Chamfer toolpath (what am I missing?)

[logicspeaks]

Greetings,

I was excited to try the Chamfer toolpath creator due to the ability to use any size ball-nose or V bits to create any size miters and I have hit a brick wall of disappointment.

Can someone reassure me?

My Issue:

I found that the creation of Chamfers cannot be controlled. Is it possible to do the Chamfer with a single pass per depth along the angle that one is cutting? Currently, from what I can tell, it pockets and clears out the material entirely several passes at every depth and this seems to me unacceptable. There is also no rest machining capability on that function which is also very surprising.

What's worse is that your Gadget is much better than this new toolpath option. One downside to the gadget is that it doesn't have the option of cutting on a particular side of the line (probably because it was designed for Cut2D) so the work around is to start the drawing of the line from the opposite side.

other software has the ability to cut any miter at any angle beautifully with the single path option and rest machining as well. So why do I care if its done this way? because the less toolpaths the less time it takes to complete the cut.

The approach to cut miters this way seems insanely inefficient. So can someone tell me if I'm missing something here?

Telling me to use the moulding toolpath is not a good alternative because this is a Chamfer toolpath and a new addition. If this isn't possible I urge you to fix this. Add a single path option (without clearing it all out layer by layer) and add rest machining like you have on the moulding toolpath.

As of now, for production purposes, this toolpath update is useless.

[mohamed]

Regarding the single pass option, you can already do that I believe by adjusting the Pass Depth and Stepover in the selected tool's settings. The number of passes is determined by those values from the selected tool.

Regarding the clearance toolpath, is this something where you'd want to use a different tool to clear out material or is mainly for adjusting the feed rates and pass/ stepover parameter on the same tool (perhaps to then have the final pass with a better finish)? Just trying to understand the use-case.

Cheers

[logicspeaks]

Let me first open up with a slight belated apology - I was and still am upset about the way this option works but I am sorry for being such a damned monster I must also add that in most ways I find this software to be some of the best on the market for its ease of use and efficient application in almost every way for a 2D program.

Now on with what you just said - I must have not been clear enough.

Here is a better way to see what I'm talking about. Imagine a miter at 30 degrees. Any miter has a slope. That slope may contain something like steps on a staircase but are actually steps along a vector. (What you're milling away is the negative space triangle).

There are two ways in this scenario to cut this. One way is to cut at a one toolpath per step (i.e. exactly like a staircase) or you can mill it away like Vcarve does it. Vcarve creates multiple passes per step and as it gets deeper there are less toolpaths per step. So what vcarve is doing is clearing out an entire layer of material per step based on the "resolution" one has specified in the tool settings as you suggested to use. (i.e. 0.05" per pass = very smooth result.)

So the higher the resolution, the higher amount of steps in both scenarios, but with Vcarves version its nearly exponential.

So with Vcarves approach this means that for every depth of cut one may be cutting 35 tool paths from the top, down to 34, to 33, etc which addes up to hundreds of cuts to finish the chamfer vs say a total of 30 passes in the normal approach.

other software and the Chamfer gadget available to users for aspire, vcarve, cut2d approach the cutting very efficiently. This is a difference of hours of cutting vs minutes or even seconds. If I'm still not making any sense the only way for you to see it I guess is to use your added Chamfer tool path update side by side with the Chamfer Gadget.

Is there something I'm totally confused about?

[adze_cnc]

While I admit that I've never used the chamfer toolpath and your explanation is a little bit difficult to follow I suspect you're not quite understanding the chamfer toolpath.

There are two ways to use it:

1. using a v-bit
2. using a ball-end bit

With the v-bit the chamfer toolpath will cut a chamfer 1/2 the included angle of the bit (e.g. 90 degree included angle gives 45 degree chamfer off the vertical). If I am cutting a 3/4" deep piece of material and specify a pass depth of 1/8" for the 90 degree v-bit in my example the chamfer toolpath will make 3 and only 3 passes around the shapes.

Using the ball-end bit is for chamfer angles that are not matched by a v-bit (e.g. if I want a chamfer 41.25 degrees off the vertical). For that matter for your 30 degree example I'd use a v-bit rather than ball-end.

This is where a smaller pass depth (such as the 0.05" suggested above) is used. This is to ensure the ball-end bit "scalloping" of the chamfer face is not too rough. In this case the number of passes, for a 3/4" deep material will be 150. Which, fine, is a lot. But perhaps a pass depth of 0.10" might be better. If I really need a 41.25 degree chamfer this is about the only way to effect it.

See this video: https://www.youtube.com/watch?v=nd3LxA5Ohbc

[logicspeaks]

I should have mentioned that we're talking about a ball-nose - not a V bit. I haven't tested a V bit and I will test that later because I'm sure I'll end up using it if needed.

But at the end of the day the usefulness comes out of the ball-nose tool-path due to the customization aspect of having the ability to cut at any angle.

So I have discovered one thing about decreasing the toolpaths and still having a rather high "resolution" via the step-downs and depths of cut settings.

My initial observation is still spot on - the way Vcarve removes material is simply confusing and just wrong - and I don't understand why its following this approach.

So I was able to decrease the amounts of cuts and keep the resolution rather high by increasing the step over to something higher than the width necessary to remove all of the material in order to have the specified miter/chamfer. (i.e. so depth of cut is 0.02 but step-over is 1 inch) But this only worked on super STEEP angles. this decreased it to exactly 2 steps per depth of cut. 1 along the edge of the miter/chamfer and 1 along the path of the bottom-most vector (the outer edge of the piece you're cutting). When you do this in reverse (75 degrees instead of 22 degrees) it doesn't work. So instead you might change the depth of cut to something much deeper but your step over will be like 0.02" it'll still be super jagged. I will at some point post screenshots to illustrate my point.

I actually have no idea how else to explain what the problem is. The only way for you to do this is to take a minute and open the chamfering gadget and then compare it to the chamfering tool added on to vcarve. Use a ball-nose and make a tool path along a square.

One program I am rather advanced in is other software, that program also approaches the cutting of the miter/chamfer like the gadget (just has many more options). It doesn't add any unnecessary tool paths like v carve at the present moment. With a ball-nose.
Either I'm totally misunderstanding something or not. So far I don't see where I could possibly be missing something.

[logicspeaks]

"other software" - so this board doesn't allow mentioning its competitors? Why censor? The competitor I'm speaking of has never removed the words "Vectric" or Vcarve from its boards.

[Adrian]

From what I can see the chamfer tool is creating a "safer" toolpath than the one the gadget creates.

With the built in chamfer toolpath it is clearing each level so the bit never has more material to cut than the pass depth specifies. With the gadget it just "staircases" down until the depth is reached. That means the bit is cutting more and more material on the side as it descends.

Now that might not be a problem if the cutting portion of your bit is as long as the depth of the cut but if it's not it's going to cause issues.

[logicspeaks]

Adrian,

Finally, someone who has actually looked at what I'm talking about. Thats fine if thats the logic they're following, but not giving one an ability to change this is a bit problematic. I forget, many people here don't use a vacuum table, nor can they afford a good vacuum pump. I am lucky that I use a 14 thousand dollar pump at work.

BUT, once you do have a hold-down that arent screws, you can cut the perimeter using a regular profile (which I did) and cut the chamfer with a single path all the way down (reducing the cutting times by nearly 200%+).

On top of it, if you're screwing things down, you can still cut a profile and add tabs. So this isn't a problem - its all about your approach to cutting the item in the right order - to force one into cutting essentially a miter/chamfer pocket into the piece at 0.03 inches at a time seems wasteful.

[logicspeaks]

On an end note to this issue - so far, it doesn't appear that what I'm talking about can be avoided with the current V11 added chamfer tool path. It is simply part of the programming. At least I know that I'm not misunderstanding something (unless I am )

Thanks for your inputs.

[Adrian]

You can still use the gadget if you prefer. It was modified to allow inside/outside cuts a while ago.

Here's a version that I've updated to work with V10 onwards as the original author hasn't been on the forum for a long time.

[logicspeaks]

Sweet! This is awesome thank you! I'm excited to take a look at it right now! Out of curiosity though - is there a section I can go into to learn how create gadgets for Vectric software? Or are they only written by vectric?

Just tried it and came up with this error.

[scottp55]

Thanks Adrian!
scott

[Adrian]

Sweet! This is awesome thank you! I'm excited to take a look at it right now! Out of curiosity though - is there a section I can go into to learn how create gadgets for Vectric software? Or are they only written by vectric?

They can be written by anyone who understands the LUA programming language. Some of the ones I've written are on the gadgets site (https://gadgets.vectric.com) and there are others from different authors in the forum section - viewforum.php?f=46

The developer info download is here - https://gadgets.vectric.com/developerinfo

[logicspeaks]

Thanks Adrian - i'll read into it - can't promise I'll figure it out but I'd love to see if I can learn it.

I posted a response edit and added that there is an error with that file. Any idea why?

[Adrian]

Sorry, forgot to change a line. Try this one.