Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

WCS probing

16 REPLIES 16
Reply
Message 1 of 17
sd-innovation
393 Views, 16 Replies

WCS probing

Hi,

 

I am preparing a CNC (Haas VF2) programm to mill several holes with counterbore in a plastic box. Because of the tolerance of the box, I need to probe the high Z for every ones.

 

So I am using the founction "new file" in machining workshop on Fusion 360 to attribute different work offset (G54, G55...). In this case I can probe every Z altitude before milling in order to optimize the machining time.

 

But I would like to probe only one time the X and Y axis for every WCS. Is it possible ? because I know that it is possible to replace the actual WCS, but I want to attribute the same value for X et Y at G54, G55... without having to probe as many time as the number of WCS.

 

Thank you in advance for your help.

 

Best regards,

 

Quentin CUNY

 

 

16 REPLIES 16
Message 2 of 17
seth.madore
in reply to: sd-innovation

Quick question; are you using a different WCS for each hole location on the part, or are you machining multiple boxes and so you have one WCS for each box?


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 3 of 17
sd-innovation
in reply to: seth.madore

I am machining two boxes (like the image) with 2 holes by box, so I would like to use 4 WCS with the same X and Y origin but different Z altitude.

 

sdinnovation_0-1712069282342.png

 

Message 4 of 17

So it is a different WCS by hole (one hole = one WCS)

Message 5 of 17

you can still just ONLY probe the Z for each new WCS

Also you can send a passthrough after your first XY probe for this 

(COPIES G54 INTO G55)

G10 L2 P2 X#5221 Y#5222;

;

(COPIES G54 XY INTO G56)

G10 L2 P3 X#5221 Y#5222;



Page 202 explains what the variables are
https://www.haascnc.com/content/dam/haascnc/en/service/manual/operator/english---mill-ngc---operator...

Please click "Accept Solution" if what I wrote solved your issue!
Message 6 of 17

Thank you @programming2C78B ! 🙂

I will try to copy G54 into G55 because I don't know how to do by using Fusion360. I will tell you news about the results !
Message 7 of 17
dlewis1000
in reply to: sd-innovation

This isn't too hard to set up but there's some considerations. Because fusion can't do specific work offsets in individual toolpaths, you have to have a setup for each hole you want to do if you want to be efficient. If you do everything in a single setup, you'll have to probe, cut, probe, cut, probe, cut, probe, cut. If you use multiple setups you can use the toolpath optimization when posting to speed things up so all 4 are probed before cutting and you're not doing extra toolchanges. If you share your file I can set it up for you. 

 

In the case of 4 setups, setup1=G55, setup2=G56, setup3=G57, setup4=G58. In each setup your probe driving WCS would be G54. You only need the Z probe in each setup.

 

In the case of a single setup, use G55 in the setup and G54 for all probe driving WCS just like above. The difference is you are going to probe one hole, cut it, then probe the next hole, cut it, etc. This way you're just updating the same G55 multiple times in the same program. 

 

Advantage of 4 setups is you then have 4 offsets that are probed every time that you can adjust individually and re-run finish passes if needed. 

 

In both cases you would manually probe G54 to locate things first and then do what @programming2C78B suggested in your program to carry over your already probed XY with G10 lines. You can do that with manual NCs I believe. Or you can just take the numbers after you probe G54 and manually copy them to G55. Then you don't have to worry about G10

 

 

Message 8 of 17
a.laasW8M6T
in reply to: dlewis1000

"Because fusion can't do specific work offsets in individual toolpaths"

 

You can do different WCS within a setup

You just need to put the toolpath/s into a folder and override the WCS

alaasW8M6T_0-1712094024191.png

 

 

No need for multiple setups

 

Message 9 of 17
dlewis1000
in reply to: a.laasW8M6T

You can set them in the probe, but not in the operations. So yeah you can probe 4 offsets in one setup, but then the toolpaths are just going to use whatever wcs is in the setup. 

Message 10 of 17
dlewis1000
in reply to: a.laasW8M6T

I spoke too soon. I never knew that was a function within a folder, I thought that was the probe setting in your screenshot. Good idea. Yeah this can be done with one setup. 

Message 11 of 17
a.laasW8M6T
in reply to: dlewis1000

Hi

 

That's incorrect, the toolpaths contained inside a folder with the override WCS will post out with that WCS

setup WCS = 1

alaasW8M6T_0-1712094591884.png

Folder WCS = 2

alaasW8M6T_1-1712094616313.png

 

resulting code the WCS = 2

14 L Z-66.327 R0 FMAX M91
15 * - Face1
16 M5
17 TOOL CALL 4 Z S700
18 ;TAEGUTEC FACEMILL
19 ;ZMIN=+0
20 L Z-66.327 R0 FMAX M91
21 M28
22 M126
23 M3
24 LBL 1
25 CYCL DEF 247 DATUM SETTING ~
  Q339=2 ; DATUM NUMBER             Folder WCS
26 LBL 0
27 M11
28 L A+0 R0 FMAX M94
29 M10
30 L X+82 Y+0 R0 FMAX
31 L Z+15 R0 FMAX
32 CYCL DEF 32.0 TOLERANCE
33 CYCL DEF 32.1 T+0.013
34 CYCL DEF 32.2 HSC-MODE:0 TA0.25
35 L Z+5 FMAX
36 CC X+77 Z+5
37 CP IPA+90 DR+ F350
38 L X+49.5 Z+0
39 L X-49.5
40 L X-74.5
41 CC X-74.5 Z+5
42 CP IPA+90 DR+
43 L X-79.5 Z+15 FMAX
44 L Z-66.327 R0 FMAX M91
45 * - Face1 (2)
46 M3
47 LBL 2
48 CYCL DEF 247 DATUM SETTING ~
  Q339=1 ; DATUM NUMBER            Setup WCS
49 LBL 0
50 M10
51 L X+82 Y+0 R0 FMAX

 

Message 12 of 17
dlewis1000
in reply to: a.laasW8M6T

Yeah I spoke too soon. I didn't know that was a feature inside of a folder. You just changed my workflow for sure. 

Message 13 of 17
a.laasW8M6T
in reply to: dlewis1000


@dlewis1000 wrote:

I spoke too soon. I never knew that was a function within a folder, I thought that was the probe setting in your screenshot. Good idea. Yeah this can be done with one setup. 


 

Yea its kind of hidden away there, I don't think many people know about it TBH

What you can then also do is put probing ops into folders, and also use the override driving WCS in the probing op to use G54 to probe G55 etc

alaasW8M6T_0-1712096834194.png

 

Good for when you have a master WCS on a pallet of parts but you want to probe each one individually the probe positions in G54 but updates G55 etc

 

Then you put each part instances toolpaths in a folder too and away you go.

 

I don't use this often myself but I don't do that sort of work really

Message 14 of 17
dlewis1000
in reply to: a.laasW8M6T

This makes a massive difference for me when doing big horizontal setups with lots of parts. If I knew about this sooner I would have saved so much time and my files would have been a lot more clean to look at. Thanks for the good tips!

Message 15 of 17
sd-innovation
in reply to: dlewis1000

Yes it is possible to create several folder in the same Setup with independant WCS. It is very useful, better than publish several Setup in one machining programm 🙂
Message 16 of 17
sd-innovation
in reply to: dlewis1000

Oh yeah thank you @dlewis1000, I didn't though to create 4 setup (one by hole) and selected all of them before publishing. I do that long time ago and it works very well ! 🙂
Message 17 of 17

Hi,

I tried your programm this morning and has I said I would give you some news about it.

It is working very well to copy the coordinates from the first probing operation to the other WCS, I just had a troubleshooting beacause I used 12 WCS and the G-Code "L2" is used from G54 to G59, for uper WCS we need to use "L20" and start again at L1 for G110 🙂

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums