[mikemill]

New CNCer attempting to make small parts, I can draw and cut them, but they get damaged as cutter comes to end of cut and parts are loose. I would like to leave holding tabs on parts, like on etched parts. Problem is when I draw tabs CAM reads as just part of whole part and cuts around them.
I have tried to write code to get the tool to 'hop' during cut on Z axis, but no succsess. Holding down parts with double sided tape does't work as not enough grip. Can anyone help?
Thanks

[HuFlungDung]

Copy your profile onto a second layer. Draw the tabs that you need on that layer.

Then, profile the part with the original layer, down to a safe level that will keep the part safely attached.

Then, create a second toolpath with the tabbed profile that you created. Cut this level all the way to the bottom of the part.

I prefer to rough the profile most of the way down with a cutter that is quite a bit larger than the finish tool. This provides a wide enough kerf that the finishing tool will not be nibbling the edge of the waste and wanting to pull it up and cause havoc. Also, you need a little bit of room to permit the tool to get in and around the tabs without descending/ascending immediately next to the finished part.

It's not dead simple, but then you are the machinist, and you have to do something to keep your elevated status

[mikemill]

Hi HFD
Thanks for advise and makes sence, but when I draw a tab the CAM sees it as part of the cutting chain and therefore just cuts around the tab and thus not holding the part! or am I missunderstang something?

Mike

[HuFlungDung]

The tab should actually be part of a continuous chain of entities which joins the part to the stock. If you close the tab off, then it is just a different part profile.

Machining the tabbed profile means that you would select partial chains, beginning at one tab and going up to (but not completely around) the next tab. Then, raise the tool, move to the other side of the next tab and select the next chain.

If your software has a shortcut for "rapid move at clearance", then you could make use of that feature. For example, in OneCNC, a certain style of dashed line will be interpreted by the CAM as a rapid movement. I do not know if this is a universal convention or not. But if it works in your software, then you can make the joining entity at the top of your tab to be a dashed line, and then you could perhaps select the entire tabbed profile, and your CAM may output moves to Z clearance at each dashed line.

[mikemill]

HFD
I understand the principle as you discribe, I am useing Mach3 with Lazy Cam.

If I draw a simple rectangle and then four tabs centerd on four sides i.e. two lines at right angles to sides lazy cam reads these lines as seperate entities.

Do I then give a smaller cut depth to the first enitie to raise tool, then origional depth on second to return tool?

Thanks

Mike

[mvaughn]

Mike, did you ever find an answer to your tabs question? If so please share it.:cheers:

[mikemill]

Hi mvaughn
I couldn't get HFD's idea to work so applied some latteral thinking i.e. if you can't raise the bridge, lower the river, by writing some extra code.
Say we are cutting a 2" square out of 1/8" material with two passes of .063, here is example of code

N4 (File square1 )
N8 (Default Mill Post)
N12 (File Posted in Mill Mode)
N16 (Wednesday, June 06, 2007)
N20 G90 G80 G40 G91.1
N24 G0 Z0.1000
N28 X-0.1150 Y1.0000
N32 M3
N36 G1 Z-0.0630 F1.00
N40 G42
N44 X0.0000 F5.00
N48 Y0.0000
N52 X2.0000
N56 Y2.0000
N60 X0.0000
N64 Y1.0000
N68 G40
N72 X-0.1150
N76 G0 Z0.0370
N80 G1 Z-0.1260 F1.00
N84 G42
N88 X0.0000 F5.00
N92 Y0.0000
N91 X1.000 to stop cut
N93 Z0.100 to raise tool
N94 X1.250 to move tool along by 1/4"
N95 Z-0.1260 to lower tool again
N96 X2.0000
N100 Y2.0000
N104 X0.0000
N108 Y1.0000
N112 G40
N116 X-0.1150
N120 G0 Z0.1000
N124 M5 M9
N128 G40 G80
M30
These extra lines of code will leave a tab connection, just add same code on as many sides as you want, allowing for were you are on x & y, on thin material with small cutter 2 tabs should hold work in place.

Cheers

Mike