There has to be a reason they are running offset cuts on the same plane . Can you Cut if the bits are at the same point of cut on Z but staggered 90degs.?

OK I cheated and made a phone call(;-).

NOW I see said the blind man.

(;-) TP

I also am starting to see the light.  So I would somehow need to modify my post processor to make this happen. That is where I will come to a screeching halt. I can stumble around in the post config files but this is probably beyond my capabilities. If there is anyone willing to help me with this let me know. I have Mastercam X2, Bobcad 23 & 24, also Vectric Aspire.

Thanks
Tom

No need for anything special. Mach3 Mill, CAD/CAM for 3 axis and 3 axis Mach Mill POST. If you try what I suggested, although in CAD and CAM (and Mach) you'll see a rather weird toolpath because it'll be in our Earthling view of 3D it'll cut just fine on a machine exactly as in the vid which is PHYSICALLY in a different universe of TWO 2D planes that share X. Try it - I just did with my standard POST and it works just fine. Here's the very rough and ready code. The Z is the roughing tool and the Y the finishing.

Ian

Ian, that is it. Now my next question is how did you combine the 2 tool path drawings into 1. I understand rotating 90 degrees but I cant figure out how you combined them. Could you post a dxf of the combined drawing.

Thank you again,
Tom

IAN you are the MAN, DAONE, you just needed a push(;-)

I had to make a phone call to someone who works on one(;-) Cheated as they say.

Seems there are 3 basic versions of these critters.

1 uses a Controller that can handle 2 planners ( very expensive. But the smoothest runningand  best quality cuts as you could easily program Arcs and lines)

1 uses a follower axis in realtime that is geared to the long axis and followes a lift table based on the long axis position. (complicated)

1 uses a standard controller and does segmented code. ( Not as smooth running , his words not mine)
THE BEST ONE he said was not even CNC it is the old hyd follower machine that used a profile plate. BUT it could not do fine detail work as well as the CNC version. you were limited by the roller follower radius.


The way they did the 3rd option Gcode was use a standard lathe CAM and draw the 2 paths on different layers and post them as 2 passes.  then he loads the Gcode in  Excell takes the second toolpass and copies  the profile axis column to a new column and moves it down to match the same offset amount as the 2 tools are offset.  He said that  a precise match up with both profiles is not essential as you are taking a rather large cut each time. Just get it close.

He also said the Cam manf wanted a small fortune to do a special post so this is what they use now.

The machines with auto loader run 24/7 only stopping for tool changes or  breaks down.

 Learn something new every day, (;-) TP 

Tom, files attached. Basically it's vector addition which you can do in a variety of ways but one way is to extrude each curve into a surface. Where the two surfaces intersect, there's the 3D toolpath. I guess it depends on whether you can do this in your CAD but you should be able to do it one way or another.

Terry, Re: the Excel idea, it's seductively simple but it's limited for the reasons you say. The problem arises because the two sets of X values can't easilly be made to match or synch. My way the two paths can be quite different - i.e. the finishing path can have more detail if you like and yet even though the paths are different they're allways EXACTLY in synch.

Ian

The way they did the 3rd option Gcode was use a standard lathe CAM and draw the 2 paths on different layers and post them as 2 passes.  then he loads the Gcode in  Excell takes the second toolpass and copies  the profile axis column to a new column and moves it down to match the same offset amount as the 2 tools are offset.  He said that  a precise match up with both profiles is not essential as you are taking a rather large cut each time. Just get it close.

He also said the Cam manf wanted a small fortune to do a special post so this is what they use now.

The machines with auto loader run 24/7 only stopping for tool changes or  breaks down.

 Learn something new every day, (;-) TP 

IT's as easy as that and it could easily be made into a VB program in Excell...
ment to write something like this but then saw someone beat me to it ;-)

Cheers

I started playing with outputting 2 tool paths and taking them into excel, when I paste the code together in the same file it looks to me that the "roughing tool path" at some point along the x axis will be using a G1 move but the Finish Tool path may have a G2 or G3. Can a single line of code have both a G1 and a G3 on the same line? I would think not.

I am thinking it my be easier to run the Finish tool path on a different computer at the same time. That leads me to my next question. Is there a way that I can have one session mach enable an output at a specific X axis DRO and have it start the program on the other session of Mach when that DRO is reached?

This project may be a little over my head so I may have to give up on it, but I hope not. I would not be opposed to paying someone to help figure it out.

Thanks for all of the advice so far.

Tom

Spunk - I've explained why this is NOT a good option.

Tom - I'm amazed at your last reponse.

Both. I guess I've wasted my time.

Ian

Ian you get no argument out of ME on this one(;-) I see where you are going with it. Can it be made to account for a tool offset like is on the machine in the VID??  That seems to be the standard approach to tooling on these things . Jonn said the offset was best for cutting. If you get the tools to close together the wood would tend to chunk out now and then. I don't know enough about wood turning to say one way or the other.

Tom on the 3rd option it is NOT done with arcs it is all micro segmented code ALL lines that make up arcs so there is never the arc problem. Probably why John said it was not as smooth running .


Just a thought, (;-) TP