Post processor edit Z0 starting point

[Fantoche54]

Hello

First of all, I must say, I'm very noob to any edit of  post-processor inside Fusion.Becose of that manyt years I stay away of the manufacture part.

I have a regular 6090 chinese router with NCstudio for my personal use.I try to use for my machine the ''NC studio programing system'' from Fusion libraryes but with the origin set at the face of the material (Z0,X0,Y0) when I start the program my machine beggin to move at the face of material to the first operation instead  of rise 10 or 15 mm and move.

This is not a safe move and sometimes drag to material.I try different post like mach 3 or generic...same thing.

Before  Fusion I use Aspire and all post have this safe retract to 10mm and move and down and start to cut.

Please if somebody know what can I do I will appreciate.

Thanks in advance

[johnswetz1982]

There is most likely an option to use G28/G53/clearance heights for positioning moves. I do not see a G28/G53 in your code but see Z13.0 called out several times so I am assuming you are using the last option. 

You probably need to jog your Z back up or home your Z axis after setting you work coordinate position before hitting cycle start.

[Fantoche54]

Acctualy i think is a missing line from PP...I try everything from Fusion WCS setting and nothing change.

Very frustrating...

[rewedesk]

Try this setting of your PP (here mach3)

 

[Fantoche54]

Thx all for patience

Unfortunately same with G28...

[johnswetz1982]

You have G28 G91 Z0.0

You need to jog/home your machine after setting your work origin.

[engineguy]

@Fantoche54 

First of all, do your machine Home setting as @johnswetz1982  has explained, and you should be OK with the G28 G91 Z0 safety line of code, you should also be able to use use the "Clearance Height" option with the modified Post Processor attached, see sample code below 🙂

'1001
'T10 D=10 CR=0 - ZMIN=-5 - flat end mill
G0 G17 G90
G0 G40 G49 G80
G21
'2D Contour2
T10
'10mm Flat End Mill
S4000 M3
G54
M8
G0 G43 Z20 H10          This line is now before the Rapid X and Y move and should move the tool to 20mm above the part Z zero you have set using the tool length offset that you have set for the tool.
X51 Y-38  X/Y rapid move to position
Z5
G1 Z1 F180
Z-4
G19 G3 Y-37 Z-5 F700
G1 Y-36
G17 G3 X50 Y-35 R1
G1 X-50 F1000
G2 X-55 Y-30 R5
G1 Y30
G2 X-50 Y35 R5
G1 X50
G2 X55 Y30 R5
G1 Y-30
G2 X50 Y-35 R5
G3 X49 Y-36 R1 F700
G1 Y-37
G19 G2 Y-38 Z-4
G0 Z20
G17
M9
M5
G49
M30

Test very carefully !! Usual Caveat applies, "Use at own risk" 🙂 🙂 🙂

[Fantoche54]

Thx. for your reply.

I don't wanna homing or jogging my  machine.Actually, my machine doesen't have homing switches...chinese job 🙂

In Aspire or Vectric cut all I have to do is to set Z0,X0,Y0 at the face of the material and when I hit start, the tool automaticaly goes up 10 mm and go to position and start plunging to the first job.

I think it's just a code line in post to do that...I don't see the point to rize manually the tool from the face of the matrial...I just wanna hit start 

Many thx to all and maybe somebody will know what I have to change in the code lines of PP

[engineguy]

@Fantoche54 

No, you don`t have to manually lift the tool up, what @johnswetz1982 is saying is you just jog your machine to a safe Z position and input that position into your Machine Z Zero Home position, you only need to do it once to setup your machine, don`t need switches 🙂

However doing it your way then :-

Check the code below, you should be able to do your X/Y/Z setting as you describe and the first axis move is the G0 Z20 which is the Clearance I set in the Operation in Fusion, is this more what you want ??

'1001
'T10 D=10 CR=0 - ZMIN=-5 - flat end mill
G0 G17 G90
G0 G40 G49 G80
G21
'2D Contour2
T10
'10mm Flat End Mill
S4000 M3
G54
M8
G0 Z20
X51 Y-38
Z5
G1 Z1 F180
Z-4
G19 G3 Y-37 Z-5 F700
G1 Y-36
G17 G3 X50 Y-35 R1
G1 X-50 F1000
G2 X-55 Y-30 R5
G1 Y30
G2 X-50 Y35 R5
G1 X50
G2 X55 Y30 R5
G1 Y-30
G2 X50 Y-35 R5
G3 X49 Y-36 R1 F700
G1 Y-37
G19 G2 Y-38 Z-4
G0 Z20
G17
M9
M5
G49
M30

[Fantoche54]

Awesome! Seems to be perfect...

All I have to risk it's just a Datron endmill and a piece of 7021 precision flat alu :))

If you ara kind...can you tell me where in visual editor I can find this string or function...maybe a printscreen...

I really want to learn how to customise my own PP.

Many thx again!

[engineguy]

@Fantoche54 

OK, if that code is good then here is a new version of the Post Processor attached for you to "play with", I don`t have time right now but I will try to find time to do a short Screencast later of what was done to the PP 🙂

You can always remove the nice piece of Aluminium after touching off ?? 🙂 🙂

[Fantoche54]

Strange....Unfortunately...in Nc studio the machine start the same way...without goes up at 10mm...

In online Gcode simulator all seems to be good..

[engineguy]

@Fantoche54 

Your code sill has the G28 line so it will do the same as before.

Did you use the Post Processor I uploaded for you and did you set the "Safe Retracts" to "Clearance Height" ????

[Fantoche54]

It works!

I hadn't set safe retract to clearance hight inside fusion.

Now all are ok.

Thx again and happy new year soon 🙂

[engineguy]

@Fantoche54 

Screencast link for you :- https://autode.sk/3q6lwFk

[Fantoche54]

Many, many thx...!

Time to play and try...maybe one day I'll help somebody here