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: 

Returning to Tool change height between WCS 1 WCS 2 work with same tool.

Message 1 of 13
667 Views, 12 Replies

Returning to Tool change height between WCS 1 WCS 2 work with same tool.

Current behavior:  

Posting part A to WCS 1 and Wcs 2 for Op1.     Tool 1 pockets on WCS 1 completes the feature,  retracts to tool change height, moves to WCS 2 plunge location, then pockets on WCS 2. 


Desired behavior:  Pocket Part A on WCS 1,  retract to Clearance height, move to WCS 2 pocket and go. 


How do I stop a full retract all the way to tool change position when a tool path instance is pattered during Posting.   I want the tool to stay down at the clearance height between WCS 1 and WCS 2 instances of the same tool path.   Any help with this?



Message 2 of 13

This is intended behavior, as it's done out of safety. Is it entirely required? No, but I don't fault the post devs for forcing this behavior.


Changing this will require a post edit, and it's not one that's handled publicly, as there is someone out there that will destroy their spindle because they aren't ready for that level of machine optimization

Seth Madore
Owner, Liberty Machine, Inc.
Good. Fast. Cheap. Pick two.
Message 3 of 13

I totally get safety..  but If I patterned the part in model mode twice, and use one wcs.. it would rapid at the clearance height between the two operations.  No less safe?


will look into a private post change.   thank you for confirming what I thought. 



Message 4 of 13

There actually is a significant difference, actually. One WCS with pattern will go to clearance plane. That's because all the parts are on the same plane. Running two vises? What if OP2 is sticking out of the vise an extra 1/2"? Or worse yet, what if you have a 3-Jaw chuck mounted on the table and a vise. The chuck is a good 3" taller than the vise. I've seen (not happen to me) what can happen when a 3" facemill plows into the side of a part at full rapid. Yes, things break.


I know @Steinwerks has a Haas post that outputs what you are looking for. I've just not gotten around to hacking up mine to do that

Seth Madore
Owner, Liberty Machine, Inc.
Good. Fast. Cheap. Pick two.
Message 5 of 13

Let's just do some quick math on this..   Not disagreeing with you at all on safety (initially).  but it's this kind of stuff that we MUST change to be competitive in a world market (coughs china)


Fadal rapids are 400ipm

let's say the retract is 15in to tool change height. 

(15/400)x 2moves x 60sec/min = 4.5 round trip cut to cut let's call it a round 5 second round trip WCS1 to WCS2


lets assume a 1 second theoretical cut to cut if traveling at clearance plane rapid 


Gives a Delta seconds of 4 seconds Per tool per part.  

For this example My part has 4 tools and when scaled into a quick change pallet will have 20pc per pallet. 


4(tools) X 4 (seconds delta) x 20pc per pallet = 320 wasted seconds 


320 seconds / 60 seconds per min = 5.33 min wasted not cutting per pallet


5.33 x ((a shop rate of $75/hr)/60) = $6.66 loss/ per hr 


spindle cost at fadal cnc. $3950  (not including labor or shipping)


$3950 / $6.66 per hr lost =  time to pay for a new spindle 593hrs. or  14 weeks of 40 hr weeks or 7 weeks of two shift 80hr weeks..   


Let's just round it and say the return on investment for not retracting to tool change height to "save a spindle"  is between 8 and 12 weeks.


for new programs I agree on safety and testing, once it's proven.. keep the tool down I'll keep my $6.66/hr in my pocket and take my chance not to crash a spindle every 8 weeks. 


Message 6 of 13
in reply to: PeterBelfanti

@PeterBelfanti Think of it more like this: if you modify the post and are running a rotary indexer and a vise, the rotary will almost certainly be MUCH taller than the vise setup (also why you see Robodrills and Brother Speedios with vise risers to minimize rapid time... but that's a different discussion), so when the tool only returns to the clearance plane for the operation and not machine home, rapids to the indexer and removes it from the table by force... things are bad. Real bad.


I understand completely why Autodesk (and HSMWorks beforehand) did this by default, and this is also why I don't share the post edit here publicly. It's not difficult, one just has to know what to look for. Since you're using a Fadal as an example, I assume you're using the stock Fadal post or a modified version thereof. I can tell you which line to edit, but again would ask that it not be shared outright, I don't want someone thinking I'm responsible for a $15k repair bill and a week or three of downtime.


@LibertyMachine I'll just send you the section. It's in every post although with more and more post changes it's getting a little more complex.

Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
Message 7 of 13

I understand your math, but I think we can both see a couple things not being accounted for:

1) How long does it take to change a spindle? So your machine is down for a day.

2) What about the cost of the part, the tool, the vise, the tool holder?

3) Have to re-setup the job. Nothing is going to be where it should have been


Your spindle is $3600. That's actually really affordable. Us folk with the new and fast machines? Add the price of a new car onto that... (My Mori is $26k. Little bit longer savings on my end) 🙂

Seth Madore
Owner, Liberty Machine, Inc.
Good. Fast. Cheap. Pick two.
Message 8 of 13
in reply to: Steinwerks

I hear your point of view totally, not arguing the liability call on the post programmer, or inexperienced programmer/setup operator..  if you have your table packed with 4 different types of work holding, vice, rotary, 4 jaw, and magic Johnson.  


My solution would be..  make this a post option check box with pop up warning messages just like multiple wcs has now, and in the header of the .nc file and work instructions..     risk it for 8 weeks, once you have the savings in your pocket.  Order a new spindle to sit on the shelf ready for the crash.  After another 8 weeks buy a ball screw to sit on the shelf waiting for the crash, another 8 weeks.. ect.  until you are pocketing money and have enough insurance on the shelf to sleep at night.   it's just a risk vs. reward call.





Message 9 of 13
in reply to: Steinwerks

That would all be valid except nearly every other CAM system does this out of the box.

Mastercam is the one I know of in particular. It drives me crazy that I cannot have this control. This is literally the function behind the "heights" tab. (In Mastercam Linking Parameters). I've used mastercam for a decade and have yet to mess this up. No reason this should be any different here. I should note the caveat of I am not switching WCS. I have never needed to, I stay in G59 or whatever and do all my rotary work in the one offset.

Message 10 of 13
in reply to: sunderlandjoe

This was driving me nuts using two work offsets and it going home all the time. I ended up modifying my haas post to allow me to toggle this on or off. Now I retract to clearance height and move to the next work offset. Saves "SOOOO" much time.

Message 11 of 13
in reply to: changedsoul

Can you offer me any insight into what you changed in your post processor to get this to happen. I would really like to save that extra time.


Thank You!

Message 12 of 13
in reply to: PeterBelfanti

@JTrudeauAURAD Its been a while since I modified it, cant remember exactly what I did, but you can try my modified post out and see if it works for you. I changed a few other things like moving the M0/M01 to after the current tool and not inside the next tool, and some other stuff.

Its been working well for me for a while now.


Message 13 of 13
in reply to: changedsoul

Thank you for the quick reply! I was actually able to solve the problem shortly after replied to you. I just found the work offset function of the post and just deleted the writeRetract(Z) line in between work offsets. This seemed to have fixed the problem for me. After I deleted that, the path will default to the clearance height rather than the retract height. 

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

Post to forums  

Autodesk Design & Make Report