Anyone use a Legacy Artisan and Conversational cam?

[myxpykalix]

Anyone here own a Legacy Artisan and use Conversational Cam? I hate the company but one thing i do like about the way they program parts is you can combine different cutting strategies to single parts. Check out this video and can you tell me what program they are using to design this part if you watch at 1:35 into the video:
http://www.youtube.com/watch?feature...v=i9nUwKrzO-w#!

I like that you can combine a "turning with a profile" or "turning with a toolpath" because cutting solely with a 3d raster seems to be the slowest. I wonder if Shopbot is going to adopt some of these turning toolpath strategies because when i had my manual legacy ornamental mill i could turn a leg profile way faster manually then on my bot on a raster pattern.

I could set it and walk away and let it work whereas i had to do the legacy manually but i can see how using the turning strategies would be way faster in the longrun.

[myxpykalix]

anyone? i'd like info on some of the teecniques they use for turning

[dana_swift]

Jack- with the continuous turning feature of the current SB3 program, I dont see anything they did that we cant make, including cutting flutes on a taper. Its great advertising, but a false claim that "other 4 axis CNC machines" cannot do equivalent things.

Flutes on a taper may require hand programming the sbp file, but I am not shy about things like that. I have not tried to make those particular cuts using wrapped toolpaths with aspire, but that may be much easier than the hand edit method.

Having an elaborate mechanism (5th axis) for the rotary axis is nice, but that axis only applies to rotary machining. Elsewhere the machine appears to be a 3 axis machine.

They also make the assertion that nothing else but their system is time efficient. They completely neglect one other metric- cost per part. If the machine costs much more than a shopbot set up for the same operations (I will make a guess its about 3X) and finishes in 20% less time (presuming this particular claim is true) then the cost per part is 3 * (1.0-0.2) = 2.4 times greater. Assuming equal machine life with my estimate for the increased cost, those increased direct costs and interest costs have to be passed along in product prices or reduced profit.

What is it you want to do that you can do now? You have posted some pretty nice stuff..

D

[myxpykalix]

Hi Dana,
I can always count on you to be able to break it down in mathamatical terms to get the simple answer. Weren't you a mathematician, or computer guy? I appreciate that...

Actually i wasn't interested in the machine (or the company) I'm a loyal Shopbot soldier, but i was looking for more information from someone who owned or used one (there are some here) because reflecting on my manual Legacy days i could make a profile way faster on my legacy then a 3d raster on my shopbot for a profile turning.

As you point out the newer version of the SB program has the continuous rotation (thanks to me, for nagging poor Ted for 2 years for it) however i haven't upgraded my program yet due to some of the problems i've seen mentioned here and because i currently can't get into the shop for any length of time because of family health issues.

But i was interested in understanding more about the sections of the video i referenced regarding their Conversational Cam programming and how they basically were drawing a part and then able to program the cutting file to that.

But getting back to the "5th axis" when you break it down it isn't anything other then a tailstock that raises and lowers with a small motor. So if you wanted to emulate that if someone wanted to munt a small stepper motor to raise and lower your tailstock that could be done fairly easily i would assume? And with talk in another post about those Wixey angle finders that might make it easy to set specific angles right?

Now here is a question that you might be able to answer mathematically. Lets say i have a 12" long blank that is 1.5" thick and i want to taper it from 1.5" round on one end to 1" on the other. No problem i can even do that with the old shopbot program...
But now i want to flute that tapered spindle. So I need to figure out the height to raise the tailstock to bring the tapered spindle to a 90 degree flat alignment with the router bit.
I suppose the easy answer is to just put a small level on the part till it is even with the bit....or just lower the bit till it is even on both ends....?

[dana_swift]

Move the tailstock? Ugh. Most likely that would ruin the setup (and the part)! Instead of changing the setup- do it with software. Wouldn't cutting the flute on a taper involve nothing more than a straight cut through space from one end to the other where Z descends from 0.75 to 0.5 while the Y axis travels from 0 to 12? A hand coded program like:

&CutDepth = 0.05 'Set the cut depth
&SafeZ = 0.5
J3, 0, 0, .75+&SafeZ 'Locate the bit above the 1.5" end of the tapered spindle
M3, 0, 0, .75-&CutDepth 'Enter the material
M3, 0, 12, .5-&CutDepth 'cut the flute to the 12" length of the spindle where the thickness is 1.0
J3, 0, 12, .5+&SafeZ 'Retract the bit from the material, repeat to cut another pass, or rotate and cut another flute

Cutting spiral flutes on a tapered is a pair of M5 commands where I show M3 with the indexer turning the angle of the flute twist over the length of the flute.

My example assumes the Z0 is the center-line of the indexer, and that the indexer is mounted aligned with the Y axis.

A real program would have a few more lines, a header and footer to start and stop the router, and perhaps do multiple passes where CutDepth increases each pass. Then rotate and repeat to cut each flute.

Cutting pipe threads on the indexer is done with a program no longer than what I just showed. As the bit descends from the entry point of the thread (a flute) the bit descends deeper into the stock (pipe) while the stock rotates. Its just too easy with a hand-coded program. I grant using Vectric products makes me think in terms of what I can draw to get the effects I want, writing a little code by hand sometimes is simpler than figuring out how to get Vectric to generate that same program.

In my case I would write a program to generate the SBP file to cut the flutes from custom parameters (I prefer C# for such tasks). Writing tool path generation programs is not particularly difficult, its just another technology, offering another set of tools to make the work easier. I have written programs like that for putting serial numbers on parts using Hershey Fonts, and another one to use the shopbot as a miter saw, cut lithophanes from JPG's, etc. Writing custom apps eliminates the need for expensive solutions from other vendors. The only purchased software I use is Aspire. It is so well done, and makes quick one-off projects as trivial as my utility programs make theirs.

My utility programs give me the benefits of Conversational Cam without any expense other than the time to educate myself. C# is a free download from MicroSoft, its part of VisualStudio Express. Start gently as C# (object oriented programming) is a huge topic all by itself, but it changes CNC as much as CNC changes manufacturing. Aspire is nothing more than a very refined object oriented program that converts drawings to toolpaths. Presumably written in C++, another object oriented language. Few of us would want to go to that much trouble, then most people want to go to a store and buy things instead of build them.

Hand coding SBP files is easy enough to learn, it makes a great place to take one step down the programming path.

Hope that helps-

D

[coryatjohn]

Dana,

Coding is a super power.

[myxpykalix]

Dana,

Coding is a super power.

I can see Dana now, in a Superman type outfit but with a different insignia on his chest...we'll call him "C++ Man"!

Dana,
I think you're right in that doing this via software instead of hardware is the way to go however unlike you I wasn't born on Krypton and don't have the super(brain)power you have.
I did it once with alot of help when i set up my spiral indexing program and no longer have the patience to even think about learning all over again.

You do have a way of breaking it down though so it doesn't seem such a daunting task.

[mick_martin]

Jack,
It's all in the tooling I run a 4th axis CNC and was also thinking if Conversational Cam would work on my machine, I bought a barley twist bit and wrote a short G-code file. I have watched there videos and and wrote my own files.

Here is part 3 where I do my finishing rounding pass using a 2" end mill then squaring up my square stock, I noticed Legacy was milling stock from both edges to reduce tear out, I tried it on my posts and it worked really good.

http://www.youtube.com/watch?v=kQrsq-9BFH4

Here is part 4 of my barley twist post

http://www.youtube.com/watch?v=tPxz8h0nRMA

Each post took about 19 minutes to cut from start to finish, starting with a 4" x 4" and 8' long post from Home Depot, very little sanding when finished machine.

[myxpykalix]

Very cool Mick...I may need to pick your brain (not your nose) on some questions i have and some ideas. What's your email address?

I made this wizard 5 years ago....
http://www.youtube.com/watch?v=jSy8PGj2eDU