[vosser]

Hi!
I'm getting ready to do my first cut. I'm however running into a little bit of a problem. When I start my Fusion 360 generated Gcode in Mach 3, the spindle jogs along the surface (Z0) to the enytry point. I would really like it to lift slightly of from z0 before doing anything at all.

I made a video explaining here:
https://www.youtube.com/watch?v=2-uBVm2Rwuc

Can anyone point me in the right direction?

Thank you.

[difalkner]

When I started I edited the file to raise Z to a comfortable level before moving to the first cutting position. Then I realized all I had to do is manually jog Z up and that's much quicker than editing the file. Now it moves from wherever I jog it - 1/2", 3", whatever - and stays that way until it reaches the starting point for cutting.

You could probably modify your Post Processor to add that line of code but it only takes a second to jog Z manually.

David

[vosser]

I thought that might be it too and tried doing that. But it moved back down again as soon as it started. I think the generated gcode is telling it to jog at z0. Although I don't see why in the Gcode.
Here is the first part of the program i ran.

(1001)
(THE SQUARE HOLE)
(T1 D=6. CR=0. - ZMIN=-7.5 - FLAT END MILL)
(T2 D=2. CR=0. - ZMIN=-2.5 - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G21
G28 G91 Z0.
G90

(THEPART)
M5
M9
T1 M6
S18000 M3
G54
G0 X70.932 Y164.438
G43 Z15. H1
Z5.
G1 Z2.5 F167.
Y158.628 Z2.297
Y157.872 Z2.271
X70.934 Y157.651 Z2.263
X71.076 Y157.521 Z2.256
X71.105 Y157.493 Z2.255
X71.398 Y157.217 Z2.241
X71.489 Y157.129 Z2.236
X71.806 Y156.804 Z2.221
X71.874 Y156.732 Z2.217
X72.194 Y156.382 Z2.2

[difalkner]

If you want to edit the file then delete the Z0

(1001)
(THE SQUARE HOLE)
(T1 D=6. CR=0. - ZMIN=-7.5 - FLAT END MILL)
(T2 D=2. CR=0. - ZMIN=-2.5 - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G21
G28 G91 Z0.
G90

David

[vosser]

If you want to edit the file then delete the Z0

Any idea how to do it by default so I don't have to edit it?

[difalkner]

I think you'll have to edit your Post Processor file to achieve that. The one I use, CNC Router Parts (Mach3Mill), doesn't add that. Z stays where I place it and doesn't go into action until the spindle reaches the starting point for the cut.

David

[vosser]

The one I use, CNC Router Parts (Mach3Mill), doesn't add that.

Hmm I just use the one called Mach3, havent changed it at all.

[difalkner]

Try this one and see how it does for you -



David

[mactec54]

I thought that might be it too and tried doing that. But it moved back down again as soon as it started. I think the generated gcode is telling it to jog at z0. Although I don't see why in the Gcode.
Here is the first part of the program i ran.

The G28G91Z0 if your machine is homed would take the Z axes up to Z0 this can be any number so if you had 15 here it would of moved up 15

If the top of your part is ( 0 ) then all you other moves should be Z- to cut your part

So do you home your machine then set your Z axes to the top of your part this is your Z axes work offset G43Z15.H1 ( H1 ) is your tool # 1 offset it is stored in the offset page so when the control sees G43Z15 H1 it is going to move the tool up 15mm

You have done your program incorrect in the cam program when you are cutting your part if you have your Tool at the top of your part as Tool Zero then all the cutting has to be Z- negative to cut the part so you have to get this part correct before you go changing anything in your post processor

[cyclestart]

If you want to edit the file then delete the Z0

(1001)
(THE SQUARE HOLE)
(T1 D=6. CR=0. - ZMIN=-7.5 - FLAT END MILL)
(T2 D=2. CR=0. - ZMIN=-2.5 - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G21
G28 G91 Z0.
G90

David

If doing that be aware G28 probably repeats at the end of the file.
In the attached thumbnail of post #7 the green text is editable, G28 can be disabled here.
On a machine without repeatable tool lengths G43 is kind of useless and potentially dangerous imo.
I delete the line "G43 Z15. H1" or change it to simply "Z15"

The way G28 behaves on your machine seems wrong to me but I am not familiar with Mach3.
Are your machine reference positions configured as the Mach3 manual suggests ?

[mactec54]

If doing that be aware G28 probably repeats at the end of the file.
In the attached thumbnail of post #7 the green text is editable, G28 can be disabled here.
On a machine without repeatable tool lengths G43 is kind of useless and potentially dangerous imo.
I delete the line "G43 Z15. H1" or change it to simply "Z15"

The way G28 behaves on your machine seems wrong to me but I am not familiar with Mach3.
Are your machine reference positions configured as the Mach3 manual suggests ?

That is correct he has his part setup wrong in his cad cam program is why it is not working as it should , Mach3 has tool offsets he just has not set everything up correct, he should not delete anything until he get his setup all working how it should be

[precisionmetal]

vosser,

Can you upload your .f3d file for this part so we can look at in Fusion ?

thx
PM