Multiple WCS

[milltechcm]

I have two setups, G54 and G55.  G54 is in one vice and G55 is in the other.  What I would like to do is run both G54 and G55 in one program and order the operations by tool.  Basically I have a set of tools that run in both G54 and G55 and I would like to minimize too changes by say facing in G54 and then facing in G55.  Thank you.

[LibertyMachine · Accepted solution]

Are both Setups in one Fusion file?

With the CTRL key depressed, select both Setups and post process them. A warning will pop up telling you that you've selected multiple setups and your post must be configured properly. Click OK. Click the button to "reorder Tools to minimize tool changes". You can than post out both programs.

Do note: You will need to make sure you define the proper work offsets for each Setup. If you leave them blank it will autofill the G54 value in the program. Not good.

Also, it will perform a G53 Z0 before changing to the next work offset. This is by design and should really only be removed if you really know what you are doing. I recall in my early days in the trade, this hotshot next to me thought he was all that and a bag of chips. Tied two programs together and didn't allow for proper retract. Drove a 4" facemill full rapid into the side of a vise. Was ugly. And loud. Very loud..

[milltechcm]

Thank you!!!

Sent from my iPhone

[Anonymous]

This combines operations, but how can we do the same thing and address the issue of keeping tool changes to a minimum?

I used to edit the gcode by hand, cut and paste.

In mastercam I would create a new operation group and copy the individual operations there,  in the order I wanted them.

Thanks

John

[Steinwerks]

Try the "Reorder to Minimize Tool Changes" checkbox on the Post Process dialogue window, should be towards the bottom left corner.

[Anonymous]

Hi

OK, that worked.

Seems like there are a lot of things in F360 that really simplify what I do everyday, by hand.

Any way to eliminate the G53 Z0. move between operations / offsets? Is that  post tweak?

Thanks

John

[Steinwerks]

Yes that's a post edit. Which post are you using? I don't like to make that edit public because it could result in very bad things with different WCS height offsets (such as moving from a vise to a rotary work offset). I'd be glad to PM you how to do it though.

[zon3sky]

Could you please PM me how to eliminate that  G53 Z0 movement between the offsets? It would  be a huge help. I often use multiple offsets and its a huge pain in the ass to always modify posted programs.

I use heidenhain posts (the generic one with little modifications for iTNC530 and iTNC 426). 

[Steinwerks]

---

@zon3sky wrote:

Could you please PM me how to eliminate that  G53 Z0 movement between the offsets? It would  be a huge help. I often use multiple offsets and its a huge pain in the ass to always modify posted programs.

I use heidenhain posts (the generic one with little modifications for iTNC530 and iTNC 426). 

---

Yes, I'll take a look at that post and PM you shortly.

[Anonymous]

Hi,

If there is any way possible I would also like to know how to change the "safe height" between WCS. I understand the dangers involved but too would like to be able to change this on a proven program where i know it is safe.

I am using the Haas - NGC post.

Thanks in advance,

Devin

[marshall.henry]

This CTRL system works but when I change tools and my CNC checks the depth of the new tool (Manual tool Change) the depth of the G54 does not update, oddly enough my G55 does update. I am not using probing. I've tried a lot of combinations to get my machine to duplicate work, but the depth's of different WCS's and manual tools have always failed. Using Mach 3 on wood/copper. Any experience with this? 

[lukerl]

I've done exactly this, and have "minimize tool changes" checked, but it still orders them by setup, not by tool.

My setup: 

I have a carrier board positioned at the origin of the machine, G54. The carrier has a one-inch grid of mounting holes and on it are three pieces of stock at different positions. One on piece of stock I machine a pattern of 3x3 parts, on the next a pattern of 7x4 parts, etc...

So I have three setups in CAM. Each uses G54, the position of the carrier, each defines the stock as the size of the carrier board but uses offset to position the actual stock where the pattern should start on the board.  Each pattern has three operations: a pocket, drilling, and a profile.

When I select the three setups and post, I get the warning about multiple WCS, I check "minimize tool changes", but the post is just each setup in order rather than T1 setup1, setup 2, setup 3; T2 setup1, setup2, setup3 .. etc

Is there anything else I should be doing? I have to go edit the file by hand to cut and paste the blocks of code into tool groups... 

[zenclaire]

Hello,

I have the same issue (see below). Could I get the answer to this as well? Thanks!

Could you please PM me how to eliminate that  G53 Z0 movement between the offsets? It would  be a huge help. I often use multiple offsets and its a huge pain in the ass to always modify posted programs.

[miguel.zambranoDULMS]

I think you can duplicate setups and order with respective tools and toolpath in the order that You want, and post process all setup that You want