Safe Z axis move

[Anonymous]

I am having a problem with the Z axis not retracting at the start and end of a g-code. The program does an X,Y move first and then raises the Z after it has cut through the top of the part. In Vectric Aspire I could adjust the code for a safe Z height. How do I fix this in Fusion360?

Note I set a retract height and clearance heights etc. in the tab and it ignores this on the first move. Using the Mach3 Postprocessor.

(BORE INDEX 1-42)
(BORING THE INDEX HOLE)
(T15  D=0.25 CR=0. - ZMIN=-0.53 - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G20
G28 G91 Z0.
G90

(CIRCULAR5)
M5
M9
T15 M6
(14 2 FLUTE)
S2125 M3
G54
M8
G0 X0.384 Y0.8158
G43 Z0.6 H15
Z0.04
G1 Z-0.015 F5.7
X0.3837 Y0.8159 Z-0.0189
X0.3828 Y0.816 Z-0.0227

[HughesTooling]

If you have limit switches and you've homed the machine the G28 G91 Z0.0 will move the Z axis to the Z home posision. What control and post are you using, on the post dialoge is there an option useG28, if there is try with it set it to no.

Mark

[Anonymous]

Mark Thanks for the response. I am using Mach3mill.cps - Generic Mach3mill.

I do not have home switches install and wonder if in that case the machine is defaulting to machine zero instead of work coordinates zero?

I will try to ref all homes in machine coordinates prior to setting the work coordinate zero and see if this has an effect on the process.

Any other suggestions?

Bill

[Anonymous]

Mark,

To answer the second part of your question.

I am using a CNC4PC C32 breakout board with KL5056 drivers and an Ethernet Smoothstepper.

Bill

[IanRobertson]

I posted about this in another thread.

I am using Linuxcnc. I do not have limit switches but before it will move I must home the machine in the software. I can then use touchoff as well if I like. The pp does have a switch to use g28 and it is set to off. I also did a 2d pocket which again sims fine but it has generated a pass about an inch over the part. I posted it for m3 and also got a funny result. Normally when you start m3 the position is 000. I opened this file and it proptly does a pass about an inch low and then raises up to follow the first pass. I hope I am doing something wrong here it can be pointed out to me. I have been running this stuff for 15 years but that does not mean I actually know anything! Don't be gentle, tell w=me what I don't know!

Cheers!

[HughesTooling]

This info might be usefull http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g28-g28.1

Also as you are using LinuxCNC did you read through this thread it's about LinuxCNC and how G53 works. I had a look at the LinuxCNC post and the useG28 option in properties just change the output between using G53 or G28 for the Z move to home. When you home the machine does it set the G53 offset to 0,0,0 and are you setting it with the Z near the top of it's stroke, can you display the machine coordinates so you can check where the machine 0,0,0 is. Are you then setting the work offset (G54) to the datum on your part so it matches the datum in Fusion, the G53 and G54 offsets should be totally independent so the G53 Z0.0 should move to the machine Z0.0 no matter what work offset you're using and touching off on your jobs should not effect the machine offset.

Mark

[IanRobertson]

Ok so the issue is that it uses the "home" position as a safe place to put the tool between actual cuts. I have not encountered this before so I was in the habit of making home and touch off the same position. All I need to do is to get into the habit of making the Z home position higher than the touchoff position. Still playing and testing but I think my tiny brain is starting to catch on, thanks.

[Anonymous]

Hey,

    Above info just saved me some mill bits.

I found i need one more step to make it work. The issue i had, and probably your having is the relative xyz. For years I would set 000 to the corner of my stock, and chop away. But this is assuming your one of the big players that has an auto home, probably 2 foot away from the massive vice. In which case there home is home, and the stock is ages away, in some random spot on the bench below, so Z0 is safe for them.

I followed above, and set my home near the actual machine home. Jogged on down to touch the stock and hit touch off to create a fake home. LinuxCNC played ball and moved the preview under the tool.

But.... After half a second, it asked for a tool change, so hit the ok button and it ploughed straight to the bottom of the stock. As now it was allowing for the tool on top of the touch off. So, with the tool in memory, stop the run, realign to your fake home, and hit 'tool touch off'. Now its actually working

Running EMC2 on a linuxCNC with some no name control box.

I think most of my toying can be fixed in emc2 such as tool lengths, to avoid the second 'tool touch off' step

Duncan

[Anonymous]

I see this being super handy if you pre drill a hole to avoid plunging with an end mill, put the hole in your CAD, set the stock point in CAM as the hole, and it will sort the rest out

[Anonymous]

Hi there, you need to modify the post processor to get the safe Z move before and going home at the end of the G-Code.

(1X6 CONNECTOR PROFILE)
(T1 D=0.2031 CR=0. TAPER=118DEG - ZMIN=-0.561 - DRILL)
G90 G94 G91.1 G40 G49 G17
G20
G0 Z1.

(DRILL1)
M5
M9
T1 M6

.

.

.

M9
G0 Z1.
G0 X0. Y0.
M30

This is how the G-Code look like after modified.

[mbelusa.mail]

Hi,

I had same issue, i hope help you with my edited post processor ....

enjoy 🙂