Help with GOROUND command please

[ImanCarrot]

Hope you can help, I know this can be done 'cos my predecessor (deceased now) done it, but for the life of me I just cannot figure out how. I've read through all the help files and Topics in the Dolphin forum so I have tried but am at a loss.

Ok the problem:

I'm milling 7 small disks out of one big disk. I only have a 2.5 axis so I have to manualy move the Z-Axis. This means it cuts round Contour1 then I have to raise the tool and the it goes to Contour2 and I have to manualy lower the tool.

Now, I know that my predecessor found a way to machine all 7 small disks at the same Z depth, ie no manualy raising and lowering the tool. It did mean going round most of the countours one and a half times though, but the whole process took about 15 mins whereas my method takes about 3/4 of an hour. I have to cut out 150 of these small parts per month for the next year so you can see my urgency

I'm using a 2mm end (slot) mill at 1000 RPM and 200mm per min with a cut depth of 1mm. Material is plastic. No coolant.

I can't upload the CAM file cos it's got a .CNC extension and won;t let me change it.

Many thanks in advance, sorry for the long post, but I desperately need to sort this.

[ImanCarrot]

Don't spend any time on this, I got a workaround. I put all the circles touching each other with one in the middle and split them into non continuous arcs. I'm now going to tell it to machine all the arcs with the central circle being machined every time one of the satelite circles gets machined. *fingers crossed!*

[John S.]

When you define the circles as contours put them all on the same group number and only these circles.
In Cam do a goround on the first circle and in Options click "Machine all contour with same group number."

even though you have only selected one circle it will cut all the rest.

Applies to any group number that is defined but, I know it doesn't matter in your case only being 2D, it will machine all the contours at the depth of the first so if you have circles with differing depth you have to program then as each or in same depth batches.

John S.

[ImanCarrot]

Thanks for that, it doesn't work on my particular application since it shoots the tool across the surface to various start points but it's a good tip to know.

I solved it by splitting all the circles into arcs and making them touch each other. I went round one of the outer circles, then part of the central circle then round the second outer circle and so on. It's as fast as (if not faster) than if I had CNC control of the Z axis.

[windy_miller]

would the 'bridge' command help? There is a tutorial of it's use on the Dolphin web site. It links different drawn objects together with a 'bridge' which the tool then follows. A good example is hot wire cutting letters out of foam where the wire needs to cut along the waste foam to the next letter and one wants to control excatly where the wire will move from one letter to the next, or circle in your case.

I don't fully understand what you are trying to do. Are these circles concentric and are they solid disks or doughnuts?

If they are not concentric and not doughnuts, bridge is the way to go. It sounds an intersting problem. Mybe you could post the cad drawing, just for interest.


Best Regards,
WM.

[ImanCarrot]

I split the circles into little arcs on AutoCad, exported that as a DXF file to Dolphin CAD, used non closed contours then bunged that into Dolphin CAM then post processed it to my turret mill and crossed my fingers.

Hehe, it worked a treat. Here's the Dolphin CNC file, watch that toolpath go! weeeeee. I love it when things work out

Proper engineering *dances about his lab*

Oh, had to do it as a Zip file cos of the attachments rules - you can't post a CNC file, so I attached it as a Zip file.

I'll look into that "bridge" command... never heard of that before, but it sounds interesting.

[Edit]Hmm nothing comes up on DCad or DCam for "bridge", perhaps my version of the software is too old? I'm on Version 7,0,0,2 L [/Edit]

[windy_miller]

Hi,

I'm usind Dolphin version 10 so maybe the older version does not have bridge. I could not actually get it to work as it should anyway.

I do like a good puzzle, so don't worry about my time spent on this. I think I have the ultimate answer

When a circle is machined, the machining start point can be set. Industry standard for the 0 degree position is 3 o'clock and the degrees then move anti-clockwise....Stay with me here....

So assuming you have a row of 2 circles, a row of 3 and a row of 2,

.....(1) (2)
...(5) (4) (3)
......(6) (7)

In the cad drawing, draw the circles as above and also draw a line just above circle 2 12 o'clock position to just above circle 3 12 o'clock position keeping clear of the circles. Now draw a line from just above circle 5 12 o'clock position to just below circle 6 position.

Set circle 1, 2, 3,4,5 up as 'start machining from 90 degrees' which will be the 12'o'clock position. Circles 6 and seven will be from 270 degrees, i.e. the 6 o'clock position

Set the two lines up as a normal cut along the line. In the CAM, machine in this order:- circle 1,2,top line,3,4,5, middle line,6,7. The machine start point will be above circle 1 12 o'clock position.

The tool will now cut the circles in the numbered order and the cutting tool will follow the line to the next row thus avoiding cutting accross the finished discs.

Regards (smugly)
Nigel.

[ImanCarrot]

Just goes to show: there is more than one solution to any given problem

Thanks everyone!

[windy_miller]

your zip file looked very pretty, the cutter wizzing about. It was more like art than cam

Hope you are well on your way to completing this months quota of 150 disks.

Get your meanie company to buy a Z axis and upgrade the sw!

[ImanCarrot]

Thank you for your kind comments, when I showed my boss the program running on the mill he just shook his head and muttered "how the hell did you program that".

Makes it all worth while hehe