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.
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Probing within CAM to establish a new coordinate system

Message 1 of 11
229 Views, 10 Replies

Probing within CAM to establish a new coordinate system

The title doesn't quite hit what I am looking to solve and if full transparency I haven't invested much time to solve the issue on my own.  I'm under a time constraint to get the quote back to my customer so looking for some help, perhaps confirming that it is or isn't possible.


I have a part where I need to start machining using one coordinate system in G54, then shift the X&Y coordinates to a new datum to drill a critical feature(reamed hole)


Obviously I can handle this using another setup.  But there quite a few parts to make and if I could use my Renishaw to move G54 then drill and ream the hole it would be a huge time saver.


Message 2 of 11
in reply to: tgford58

Make it a second setup.  At the end of the first operation (g54)  add the probing but do it to coords 2/G55. Second setup base it on the G55 you just made.  (Don't forget Z if you aren't doing it in the program.    Then you can post the two ops together and as long as your post is cool then it works.  



Message 3 of 11
in reply to: tgford58

I think you could do this with a folder. Setup>New Folder. Right click > Edit > Post Process > Override WCS. Then put your drilling/reaming toolpath in the folder.


You can keep G54 for your original datum, and use probe WCS to reference G54 to move to the ideal G55 WCS and probe for and overwrite the exact location.


If you change the drilled hole to G54, you need to re-probe your original datum every part. 

Message 4 of 11
in reply to: jonathanBUCVS

@jonathanBUCVS   Ok I am intrigued.   I have no experience with folders.  Can you briefly explain what they are and how to use them?


I learn something new with Fusion everytime I use it and the community is the benchmark for users helping users.


Thank you for your time.

Message 5 of 11
in reply to: TrollTuner2

@TrollTuner2  So this way would 'automate' establishing the G55 WCS?   How can I imbed the 2nd OP within my post?  I think that is what @jonathanBUCVS is alluding to.  I wish I understood folders better.

Message 6 of 11
in reply to: tgford58

There are 3 things you can do with folders (that I know of)

1. Use them like regular folders for organizing toolpaths. Not very exciting

2. Use them to make patterns of toolpaths that are in the specified folder

3. Use them to change the WCS on specific toolpaths that are in the specified folder. 


You cannot organize Setups with folders. You can only organize toolpaths within a setup. 


If you want to do two setups, the easiest way to post both OPs together is to just select both setups when you post them. You cannot embed one into the middle of the other this way. 

Message 7 of 11
in reply to: tgford58

You don't really need to change which datum you use, as far as i can see. 

Say you have a square milled outside profile and you want your hole dead nuts in the middle, you just mill the outside, probe and reset your g54 on the outside you just milled, then drill and ream at some X and Y coord from that.

Message 8 of 11
in reply to: wstoneandsons

@wstoneandsonsThat is exactly what I am trying to do.  Op 1 mills the periphery and top of the part and adds features, G54 is top dead center of the stock.  What I want to do is have the last tool drill a hole using the back left corner, top as its origin.  This feature is measured from that point and is pretty tight on tolerances.

Your way is valid, if I understand correctly it requires a second Op.

Message 9 of 11
in reply to: tgford58

Its only a "2nd op" in the sense you make it a seperate Setup with a different WCS and origin. You still post it out at once, resulting in 1 code file. 


op 1: mill, measure g55 corner
op 2: ream hole based off corner

Please click "Accept Solution" if what I wrote solved your issue!
Message 10 of 11
in reply to: programming2C78B

@programming2C78B @wstoneandsons @jonathanBUCVS @TrollTuner2 

Sorry for the delay in responding.


I've attached the model and code for what I am trying to accomplish.  I've posted to Haas NGC but I am just not knowledgeable enough to sort through the Renishaw Macro calls.


Any help that the group can provide is appreciated.  I just want to have a probe after I run part 1.

Message 11 of 11
in reply to: tgford58

First you need to separate it, with a Setup for Offset #2 (G55) with the proper location. 


You also need to override the WCS of the probe operation by putting it into a folder with an override.



then post these both out at the same time. AFAIK when you probe it like this though, it'll put in the g55 value of the model center again. It probes the corner, and applies the offset of 1/2 your model to make it match your setup folder. Youll want to actually probe it in setup 2, and could use a passthrough to apply an offset to make it work. 

FYI, if you just mill your part OD to exactly nominal, you can still hit that positional hole callout without having to probe the milled corner. The location will still be correct. I do this on any .001" positional holes, and as long as your OD is within .0005" you're good!

Please click "Accept Solution" if what I wrote solved your issue!

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

Post to forums  

Autodesk Design & Make Report