Use Fusion 360 to automate and reduce setup time with override driving WCS 

Hi Kurt, yes its a different midset to get in with this workflow but once you get it working its a real time saver, you can swap jobs out all the time and never have to manually set up.

Then you don't have to manually probe the part. Once the G59 is set, you model everything up in Fusion and then let the machine do the probing automatically.

I think its for people that program all their parts using all the fixturing. So if you have fixture "C" and the zero point is 5" up from the never moving part of the fixture (G59) the probe knows where to go on the first part. I really dont see it as that much of a time saver. Its only saving you from probing the first part, after that, they are all in the correct place. Everybodys got their way though.

Hi @Crivo 152 The issue with setting G54 and then using G54 is it is constantly moving from part to part. Its good practice to have a static datum that the part relates back to. This is really useful for multiple part production. If you use the action "out of position" to alarm if the part is too far to out in X for example. You will be checking is this part within tolerance from the last part. This can cause variation and creep. If the part was to move 0.5mm to the left every time, after 10 parts its now 5mm out. If you use override driving WCS every part comes from a static datum so part 1 is 0.5mm out, part 2 is 1mm out and so on. So setting out of position alarm at 0.75mm would not alarm in the first case, but would alarm with override driving WCS.

@@richardstubley9651 Thanks Richard, I guess It is hard for me to understand the gains since I only have a homemade CNC mill and I don’t run batches of parts. Things might change in the future though, so I am keen on learning everything I can. I genuinely enjoy the tips these type of videos provide.

@@vilts This answer is the simplest and best in my head. Thanks!

Probing a WCS in a 5-axis setup is pointless and retarded, as once you move your origin out of the point where the A and B axes intersect, parts come out wrong because it's been moved in a way Fusion did not expect. A 5-axis table needs to have a constant origin point in the centre. You can use probing to inspect a part, but never to change WCS in a 5-axis!

@@duodot I assume you didn't know about MSRP and DWO 2 years ago?

Yeah I'm trying to figure out the same thing. How do you tell Fusion where G59 is?

@@SteveN-bh3wv Look at my reply a little lower, I go into more depth on how to get Fusion to actually find the right G54/G59 combo.

Hi @Daniel this works exactly the same on a Heidenhain, It was actually a project I did with a customer on a Heidenhain that made me make this video. On that project we used Pre-set 40 as the static datum and then pre-set 1 as the local datum that was updated for every part.

@@richardstubley9651 It seems that it might work as intended :) I haven't double-checked yet, but is it possible to use preset 0 as the one that updates? That one is the one that is used as "default" and gets updated when you set wcs from manual-mode (in some cases at least) We use presets for reccuring parts to speed up setup-time. We have the stock-size defined in our setup-sheet (or you check it inside the project-file) In our case we dont want to move the WCS around for every part when running automation. But we want a simple way to automate when we run one-offs and setups a new recuring job

@ this method sounds like it will work perfectly for you then! When I did this on a TNC 640 we didn't use preset 0 we used 1. Looking at the manual 0 can do things a bit differently so we didn't risk it. I'm sure 0 would have worked but it was just as easy to use 1.

I've got this issue as well. I think it's a "feature" of F360 and the Renishaw probing cycles. When I follow this video the probing cycle and subsequent tool paths work as expected, however, the G54 is updated more as an error offset from G59 than actually updating G54 to the desired point. As an example, our G59 is at the back corner of the vise and we want to drill a hole in the center of the part with the G54 WCS located at the center as well. Let's assume the part is 6 x 6, and the vise is fixed jaw and is also 6 in width for simplicity. What Fusion will do is use the P9812 (web measure) Renishaw macros to find the difference in reference position, honestly it's more like a G52. Below is an example output for finding the X and Y web reference. N10 G59 (Static WCS assume 0,0,0) N20 G01 X3.0 Y-3.0 F400 (move to part EXPECTED center in reference to G59) ... (turn on probes, and protected moves) N30 G65 P9812 Z1.5 X6.0 R0.5 Q0.5 S1 (Measure X web, save to WCS=1 'G54' ) N40 G65 P9812 Z1.5 Y6.0 R0.5 Q0.5 S1 (Measure Y web, save to WCS=1 'G54' ) ... (turn off probe and protected moves) ... (switch to drill and set tool height) N50 G54 (Actual WCS) N60 G00 Z2.5 (assume this is 0.5 above part) N70 G01 X3.0 Y-3.0 (move to the EXPECTED center position as programmed from G59, and compensated by G54) N80 G81 Z1.5 F20.0 (drill cycle) What happens on line N30 and N40 are the renishaw macro calls for web measure. The important bits to look at are the X and Y values. In the Renishaw macro it wants the "nominal size of feature" in X or Y axis. And remember the probing cycle will give the "Difference in expected position". Since we know nothing of G54 it has to be in reference to G59, so our expected center point is X3.0 Y-3.0 with an expected web thickness of 6.0 in X and Y. Let's assume the stock is centered in the vise but actually 6.1 in X and 6.2 in Y in size. After Running line N30 and N40 G54 X will be updated to 0.0, G54 Y will be updated to -0.1 (we'll omit Z). X wasn't updated because the material is centered in X, but Y is changed to -0.1 because the material is 6.2 and the vise is a fixed jaw. So the key here is the DIFFERENCE of the expected and actual in reference to G59. In the Y direction the expected center (from G59) is -3.0, but because the material is 6.2 in width the ACTUAL center is -3.1 from G59 (remember we have no idea where G54 is). So the following lines for the drill operation use the expected center position from G59, but we use G54 to compensate for the difference. And I agree that it's not the expected solution, you'd expect that because you probed the center of the part the center of the part should be X0.0 and Y0.0, and not X3.0 and Y-3.0. Hopefully that makes it clear as to what's going on. The feature is more like using G52 offset than actually updating G54 to the TRUE WCS desired. SO be careful with subsequent setups that use G54 and the part center as the WCS, because if you don't probe with override WCS you WILL CRASH. Because G54 is at the difference of G59 from expected. To get around this, and I should probably do this as well, is to use the macro variables for G54 WCS (For Haas NGC) #5201-#5206 and Fusion with manual NC to update the G54 part position center in relation to G59 as a parameter and then probe the ACTUAL G54 part center point since we now have and expected ACTUAL reference to G54.

I decided to make a macro for Fusion, it wasn't too difficult, it makes the following lines to update G54 based on the G59 point in space so you have a start reference, and creates a manual NC. You could just as easily create the Manual NC operation and paste in the below for Haas NGC, then manually change the values based on your setup. N20 #5221 = #5321 + [0.0] (Update G54 X from G59) N25 #5222 = #5322 + [-2.0] (Update G54 Y from G59) N30 #5223 = #5323 + [2.015] (Update G54 Z from G59)

@@capnthepeafarmer wow this Macro is a beautiful thing. Thanks for your response, I really enjoyed reading it I absolutely love this stuff and it's rare to find someone who speaks the same language, especially with the advanced stuff. So I had actually contacted someone at Fusion a few months after this comment, and after arguing with the poor guy for far too long he helped me come to the conclusion you outlined above. The worst part is I realized I was wrong when he said "did you try running a program after using the cycle?" To which I replied "of course not! I'm not gonna run my program when the offset is clearly incorrect everytime I check!" Long story short: I overcomplicate things so often it's almost unbelievable. I was so certain it was going to update G54 in the expected way that when it didn't I just figured there was something wrong with the cycle. I'll check out that macro next time I get a minute, I had intended on making one myself at some point but just haven't had time so thank you kindly for sharing your solution.

@@RyanM33 No worries! Coming from SolidWorks and MasterCam, there are a lot of things I expect out of Fusion 360 that are absolutely trivial in other programs, and it drives me nuts. And the only way I have been able to get around those limitations is to learn how to do scripting in the Fusion API (which is super easy). The API has its own limitations, but at least you're able to kludge it in the background behind a button press 😂

@@capnthepeafarmer so in the manual when it says "New work offset = active work offset + error" I expected that the G54 would be calculated as as follows... Let's say G59 is 10X,-10Y (machine). Wouldn't G54 then become 13X,-13Y (machine) after probing since G59 is the "active work offset" and G54 is the "new work offset"? Then the drill operation would be called as X0,Y0 (G54)...That's how I expected it to work. Would be great if you could set a probing reference (ie G59) then probe and set your target work offset explicitly, having both coordinate systems on the screen, with the probing reference depicted as a different icon. I get that it's basically making G54 an offset from G59.

Not all machines use G54-G59 And one of the strengths of CAM systems is the ability to change the machine you are posting to without having to re-do everything. So we choose the most universal way to display this. 1=G54 on a HAAS 1=1 on a Heidenhain 2=G55 on a HAAS 2=2 on a Heidenhain and so on.....

0 = G53 , machine origin !

​@@getsix10 Be careful a lot of our posts are configured to use 0=G54 & 1=G54 as its extremely rare people program from machine WCS inside of CAM systems.

@@getsix10 No, both 0 and 1 is G54. G54 is 0 by default, unless you use a different WCS, whereupon G54 is now 1. So G55 is 2 and so on.

@imfbrad, the whole idea here is to leave a datum static that never changes. So you can rely on this from part to part, if you didn't use this that datum would be constantly changing and may change to a point that can cause issues.

@@richardstubley9651 doesn't make since if you have to probe G54 there is no point in the G59. Its pointless. I have been doing this for over 25 years and doesn't make sense to me. If you were saying there was no g54 then it was make sense better

@@imfbrad it does make sense if it's possible for the stock or part to vary slightly in size or position from one run to the next.

@@ScottMoyse If that is the case the g54 would do the exact same thing.

@@imfbrad You're wrong. Imagine setting up ten parts on a 3-axis bed, all referencing the same hardcoded datum. You can line the programs up and let it probe every location while you walk away to do something more valuable. Moving your datum probing to a repeatable, dependable process is a massive win for reliability and productivity.

Hi Sorry about the weak audio, I try and do these live in the shop rather than just behind a PC screen, that does unfortunately mean lots of background noise, we do filter it out but its never as clear as sitting in a sound booth. As for the accent, not much I can do about that :)

@@richardstubley9651 the audio was fine mate. Accent spot on. Thanks for creating a great video that clearly explains why and how it works.

@par4par72 there's far too much barking and terrible music in the single video you've posted on your channel. 👍.