Ok, I give up. 7 start thread

I lied. Thought I had it, but it's threading from z minus to z positive. That's for a left hand thread.

If I switch to RH thread it works correctly.

I'll keep trying.
 
I see nifty creations like this and I really would like to score a smallish machining center and dive back in.
spumco said:
Yes, F360 supports live tool mill-turn. These were done using F360 CAD and CAM on an Emco 325-II

Don't know if the new Hobby license rules cripple mill-turn, however (I'm on a Startup license).

View attachment 342493

And Jim's right - F360 CAM threading doesn't require any threads on the model. You could model a cylinder and all the cutting variables are set in CAM. The threads in the screenshot below are not modeled - just there for reference.

View attachment 342494
Click to expand...
 
alloy said:
I lied. Thought I had it, but it's threading from z minus to z positive. That's for a left hand thread.

If I switch to RH thread it works correctly.

I'll keep trying.
Click to expand...
Dyslexic drawing? :big grin:
That is something that would happen to me if I were to try.
Keep hacking away at it. It'll come together all of a sudden.
 
alloy said:
I lied. Thought I had it, but it's threading from z minus to z positive. That's for a left hand thread.

If I switch to RH thread it works correctly.

I'll keep trying.
Click to expand...

That's what I did, set it for a right hand thread, then edit the G code to set a clockwise spindle.
 
Ok that makes sense now. I'll give that a try.
 
Here is a bit of the code.

I see on lines 20 and 22 and so on the feed is" F0."

Is this normal?

Does it have something to do with this?

I'm trying a feed of .120 this time.


(WHEN USING FUSION 360 FOR PERSONAL USE, THE FEEDRATE OF )
(RAPID MOVES IS REDUCED TO MATCH THE FEEDRATE OF CUTTING )
(MOVES, WHICH CAN INCREASE MACHINING TIME. UNRESTRICTED )
(RAPID MOVES ARE AVAILABLE WITH A FUSION 360 SUBSCRIPTION. )



%
O1207
N10 G98 G18
N11 G20
N12 G50 S500
N13 G28 U0.W0.
(THREAD1)
N14 T0505
N16 M8
N17 G99
N18 G97 S200 M3
N19 G0 X1.81 Z0.1969
N20 G1 Z0.805 F0.
N21 X1.7953
N22 G32 Z-0.625 F0.07874
N23 G1 X1.81 F0.
N24 Z0.805
N25 X1.7807
N26 G32 Z-0.625 F0.07874
N27 G1 X1.81 F0.
N28 Z0.805
N29 X1.766
N30 G32 Z-0.625 F0.07874
N31 G1 X1.81 F0.
N32 Z0.805
N33 X1.7513
N34 G32 Z-0.625 F0.07874
N35 G1 X1.81 F0.
snip
 
Hmmmm, that's not going to work very well. Looks like they really broke the Fusion free version. By eliminating the rapids they broke the threading function. You can't set a feed speed for a threading tool as you could for a turning tool.

So the fix is to replace F0. with F30. (just to keep things kinda slow for testing) I use notepad for this, use the search & replace function.
 
Ok, mastercam has a good search and replace function.

I replaced F0.07874 with F.07874, then replaced F0. with F30.. Otherwise it replaces everything with an F0.##### with F30.

I'll give it a try soon.
 
You must log in or register to reply here.
Back
Top