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: 

Probing and Updating WCS for Angle

17 REPLIES 17
SOLVED
Reply
Message 1 of 18
alan
1976 Views, 17 Replies

Probing and Updating WCS for Angle

Hello,

 

I'm machining a casting that has an existing pocket.  I need to radius  where the pocket meets the top flat surface.  Because they are castings there is no surface to use a s a line up guide.  I want to probe the pocket for location and one wall to set a G68 rotation angle for the control to use so I don't have to line up each casting.  The machine is a Haas.

 

When I set everything up in Fusion I get this warning when I go to post process the program.

 

Error: You cannot probe while G68 Rotation is in effect.
Error at line: 1550
Error in operation: 'Probe WCS12'
Failed while processing onSection() for record 955.

 

I have attached the error file.  What do I need to do so I can achieve what I described.

 

Also attached is the Fusion file i'm working on.

 

Thank you for any help.

17 REPLIES 17
Message 2 of 18
Richard.stubley
in reply to: alan

Hey this was a nice and easy one.

 

You cant probe once you have g68 active, so just change your order around so that your angle probe is the last one out of 3.

new order.png

 

Also while you have free access to the manufacture extension give inspect surface a go!

 

Setting Inspect Surface on a HAAS Classic

https://www.youtube.com/watch?v=N5naayLBr7g&t=379s

Setting Inspect Surface up on a Next Gen

https://www.youtube.com/watch?v=d9VnOJoQbvg&t=106s

 



Richard Stubley
Manager - Manufacturing Specialist Team
Message 3 of 18
alan
in reply to: Richard.stubley

Thank you.  That solved the issue.

 

I am confused about "while you have free access to the manufacture extension".  My subscription has always had the manufacturing extension.  Is something changing?

 

Thanks Again.

 

Alan

Message 4 of 18
Richard.stubley
in reply to: alan

Hi @alan,

Do you mean you have always had access to the manufacture workspace?

 

The manufacture extension is a addition level of functions above the normal manufacture tools. Steep and shallow toolpaths, in process inspection capabilities, hole recognition to name a few.

 

The extension is normally purchased with cloud credits 30 days at a time, but is currently free for users.

https://forums.autodesk.com/t5/fusion-360-manufacture/extended-access-program-free-fusion-360-commer...

 

 



Richard Stubley
Manager - Manufacturing Specialist Team
Message 5 of 18
alan
in reply to: Richard.stubley

Richard,

 

Thank you.  How much is the extension?

 

Back to the WCS angle.  Does Fusion automatically write the angle to the Offset?  I believe I need to get the angle value to macro #168.

Message 6 of 18
alan
in reply to: alan

One more issue.  When running the Contour part of this program the plane changes from G19 to G17 and back to G19 which is illegal with G69 rotation enabled.  The contour is actually a chamfer.

 

Do you have a solution for this?

Message 7 of 18
alan
in reply to: alan

Hello Richard,

 

Do you have a solution?

Message 8 of 18
Richard.stubley
in reply to: alan

Hi @alan,

 

Sorry had yesterday off and saw this on my phone so couldn't open the file to check. 

 

If you take off the vertical lead in radius this should stop the swap in plane selection.

 

vertical lead in.png



Richard Stubley
Manager - Manufacturing Specialist Team
Message 9 of 18
alan
in reply to: Richard.stubley

Richard,

 

No need to be sorry, you have been very helpful.  It all works perfect, updates the angle and everything.

 

Thanks a ton.

 

Alan

Message 10 of 18
DarthBane55
in reply to: alan

Every now and then you pickup a trick in this forum, and this one was the trick of the day for me!  Thanks for posting your issue, and for the answer as well.  I posted this with my post and it works, then looked up the renishaw manual and saw that cycle, very far in the manual, didn't realize this was a cycle up to now...  I did this exact task before by probing 2 points and doing some math with the resulting variables to get the angle!!  I should have read the manual more in depth...  Feeling dumb... 😯

Also a little trick for you, in case you didn't see it already...  when you probe the pocket, your probe retracts between each moves because you picked the cycle with island.  Change it like picture below and the probe will stay down, saving just a bit of time.

1.png

Message 11 of 18
alan
in reply to: DarthBane55

DarthBane55,

 

I'm glad this helped you too.  This forum and the Auto cad employees are great!!

 

Thanks for the pointer on the rectangle without the island.  I will change my routine.

 

Thanks Alan

Message 12 of 18

This works to probe a single feature that requires a G68 rotation, but only one, because apparently the Haas NGC post doesn't un-set rotation with a G69 after the probing operation is done?

This seems like a misfeature to me. 

Message 13 of 18

Hi @markaudacity,

 

The idea we have behind the use of this is that we probe a feature to set the G68.2 angle, then you mill the pat with this active. If we were to cancel the G68.2 with G69 then it would not be active for the subsequent milling ops. 

You cannot probe with G68.2 active so always make sure angle probing is the last probing op you do if you are doing multiple probing ops. 



Richard Stubley
Manager - Manufacturing Specialist Team
Message 14 of 18
Anonymous
in reply to: Richard.stubley

Hi @Richard.stubley 

I've ran into this issue today:

 

Error: WCS offset cannot change while using angle rotation compensation
 
I run a Haas UMC750ss. I have two workoffsets in my program and I align G54 and this operation changes my C-axis workoffset (not G68). I think it's more than logic when the post switches to another WCS it will retract in Z and then rotate.

Any tips on this?
Message 15 of 18
Richard.stubley
in reply to: Anonymous

Hi @Anonymous 

As far as I'm aware in the post as long as there is a C axis available it will use that as a preference over G68.

So if you have a C axis enabled it will  update the C axis value in the WCS table, if you do not have a C axis enabled in the post then it will use G68.




Richard Stubley
Manager - Manufacturing Specialist Team
Message 16 of 18
Anonymous
in reply to: Richard.stubley

Yes it does update the WCS C-axis. But look at the error, I can't run G54 and G55 in the same program when I do a 'along Y axis alignment' in G54.
Message 17 of 18
Jools-Taylor
in reply to: alan

@Richard.stubley 
I'm trying to utilise this on my Syil X7 machine at the moment. Or should I say we're making the post processor implement this but I have questions/clarifications

There is no 'output to G68' option on the dialogue boxes when you program a probing cycle. Is it therefore only true that it automatically outputs a G68 code if you do an 'angle along surface operation'? Please explain how this works or if other things are required.

Is that the only way to calculate an angle of rotation? I have a cylindrical part I need to machine top and bottom There are only 2 bores that penetrate through the part (I.E. machined in op1 and visible in op2). Is there a way for fusion to probe the centres of those 2 bores and use the two centre points to calculate the center of rotation? 

Can the probing functions output to macro variables? In example one above I could run two probing cycles, store the respective coordinates and have the control do the maths. But I can't see how to do that. Can you suggest anything?

regards

 

Jools

Message 18 of 18

Hi @Jools-Taylor,

1) Currently we can only set angles by probing 2 points on a face, the post processor then either applies this as a G68 or C axis rotation.
We currently don't support a macro to do an Angle between 2 holes.

2) We are just calling macros in this case so it's completely dependant on if the macros on your controller expose the results for you to then store in macro variables.

You could use part alignment to measure the 2 holes and then use the surface points to align from there but that will involve re importing the results to calculate the shift and then re exporting the new NC code.


Richard Stubley
Manager - Manufacturing Specialist Team

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

Post to forums  

Autodesk Design & Make Report