Turning Canned Cycles and Fusion?

[LibertyMachine]

After a bunch of searching on this forum as well as the Post Processor forum, I've come to the realization that there isn't much in the way of support for Turning Canned Cycles, such as OD/ID Roughing or Finish canned cycles, threading, grooving so on and so forth.

Question is this: Is this a function of the Fusion software, or is it current limitations of the Post Processor?

If it is software, where does it land on the development roadmap?

While I do not currently own a CNC lathe, I was trying to get some code out for my employer (day job) and I ran into that unexpected limitation. 

Comments from the developers?

Side note: if one was to buy an older used CNC lathe, the memory capacity could very quickly be absorbed by a program of medium complexity, assuming more than a few tools. Yeah yeah yeah...drip feed.

[Anonymous]

it is impossible fusion360 allready generate toolpath before post. its worthless.

i write gcode faster than cam.part allready done and packed sended customer before there is single line post processes.fusion360 is for hobby machines that cant use G2 G3 G70 G 71 etc..yeah who would pay software like that. its faster handwrite.just type measures from drawing DONE

---

[Anonymous]

goodluck for that. there is no need create tool path. just one pass and post process do job. no RED RED RED COLLISION. i would pay dollar if it do G71 lol. i allready done it. buy post processore 1 million? make more sells?

[LibertyMachine]

@Anonymous 

If you are having that poor of a time using this rather decent piece of software, it sounds to me like there may be a carbon based error at play....

I could point you to many professional shops that use this software on a daily basis, but I suspect you really aren't that interested in hearing an objecting point of view.

Is turning in Fusion lackluster? Yeah, it is. Is the team working hard on improving that? You betcha.

[Anonymous]

Where there is a will, there is a way. You can generate only finish pass using insert you intend to rough with, don't leave any stock.

At the machine, just type in your one or two line canned cycle and arrange finish tool path you generated so that it is between blocks corresponding to P and Q parameters in canned cycle example below.

G0 X2. Z.1

G71 U.1 R.02

G71 P101 Q102 U.01 W.005 F.012

N101 GO X1.

G1Z0

X1,1 Z-,05

N102 X2. Z-3.

GOZ.1

Guys at the machine should have full understanding of canned cycles functions, rules and limitations.

Canned cycles are listed in books supplied with machine tools, there are free PDF files on web with all the "secrets" spelled out as well.

I couldn't imagine working without canned cycles.

It should be top priority for Fusion team because roughing 20 inches diameter part is not practical using point to point passes, besides saturating machine memory with endless pages of code, fine tuning cutting conditions can be a nightmare with reposting just to change depth of cut.

If pecking is holding you back, there is a way to deal with that too, divide area to be roughed into segments and use G74 cycle for axial or G75 for radial roughing using as many cycles as it takes to remove stock then follow with one or two semi finish passes to remove stares and leave uniform stock for finish pass with another tool.

I, as a programmer decide how to handle the task, if tool is not there to help me with that, I look for one that works, in most cases I get away with $150 worth editor with some 2D CAM features that let me draw part profile and generate finish pass over desired segments, that can also be easily reproduced in Fusion.

In Fusion we have ability to generate sketches which means we can outline what we want to cut then employ techniques that produce results, insert comments and finish posted program in NC editor by inserting templates, cut and paste, delete one thing and add another ...... yes you can produce canned cycles in Fusion but it is not going to be driven by menus and preconfigured features, you must be the one to do it until that becomes available.

[Anonymous]

i know how write canned cycle. i know my part measures. those go in cycle,
question why i need fision360 it not make things faster. annoying long code

[Anonymous]

I have been using canned cycles for past 30 years, along with that I have been using any CAM package that I could get my hands on and there is valid reason to have both.

Canned cycles are limited in what they can do just as anything else. It's easy to punch in few lines and start making chips but efficiency is another matter when you have more complex part than strait lines and boxes. 

For example, Fanuc G71 type 1 canned cycle does not allow undercutting, so if you have cavity to machine your choice is G71 type 2 which in my 30 years I have not seen used more than few times by all my peers including myself.

Next option is G73 which will cut as much air as material and I have seen people mess with parameters to the point of crashing tool into the part because most did not understand how stock is divided into desired number of equal depth passes.

Now, assuming we are all fully aware of how things work, best way to get things done is to use canned cycles where they have advantage and use long hand programs where there is a need, like deep undercuts and grooves where grooving tool is not best choice but 30 degree profiling tool is.

Many possibilities there so I need all options and know how to use them before dismissing them entirely.

So the real question is, how fast can anyone beat good CAM system in accuracy and efficiency of creating tool path that details pockets and contours canned cycles are just not suited for ? 

If CAM systems were useless, no one would be striving to create and refine them.

If canned cycles alone were all we needed I would not have witnessed so many busted tools and crashed machines over the years because those experts just couldn't see it in their crystal ball soon enough to prevent them, clouded by so much confidence that they insisted on not using tools available to them, such as CAM or back plotting code before running it.

There is a software on the market that will accurately back plot NC programs using canned cycles, it will show same activity as when program runs in machine, so you can debug programs before crashing.

I assisted in creation of it and I use it because it catches  mistakes before it's too late.

One more thing, those accidental crashes mostly involve people crashing someone else's machines and tool holders then moving on to another job where they further "developed" their skills at someone else's expense.

I use CAM software and canned cycles selectively,..... both have valid and unique benefits but I do understand freedom of choice, ... so long as there is undeniable advantage in doing so.

[akash.kamoolkar]

@Anonymous 

You make a great point about machining undercuts with canned cycles. My team is working actively on implementing turning canned cycles into Fusion 360. Currently the intention is to implement them in such a way that they will be able to also machine undercuts (as best as they can) by recognizing these features and making sure that the profile points passed to the controller are gouge free and do not cause any crashes / tool breakages.

Regards,

Akash Kamoolkar

[CAMXPRESS]

Hello Akash,

Do you have any good news for us about the project?

Regards,

Joe

[andrew.todd1]

Yes, this news would be very welcome!

[akash.kamoolkar]

@CAMXPRESS @andrew.todd1 

Hey guys, we are putting the finishing touches on the canned cycle development and also working with our post processor team led by @GeorgeRoberts to make sure our turning post processors will be able to support canned cycles. They will be delivered soon in an upcoming release.

Regards,

Akash Kamoolkar

[scottmoyse]

@akash.kamoolkar can we get a sneak peak? and provide feedback on it before release etc?

[akash.kamoolkar]

@scottmoyse we're still working on implementing the post engine side and post processors for the canned cycles. Receiving feedback on them would be very helpful but we feel it's too risky to put them under a public feature flag until we've tested them rigorously. Once we are satisfied they are ready to go we can release them with the new strategies.

Regards,

Akash Kamoolkar

[scottmoyse]

But what if you do all that work and it's not what your users want?
Kind Regards
Scott Moyse
Manufacturing Technical Specialist Autodesk Expert Elite
P: +64 9 302 4028 M: +64 21 055 7775
[email protected]

CADPRO Systems Ltd
Auckland - 527b Rosebank Road, Avondale Auckland
Christchurch - Unit 3, Kendal Avenue, Burnside
New Zealand

[daniel_lyall]

@akash.kamoolkar  do it under the white list

[Anonymous]

Thanks good reply. and yes my engluis suck :))

G71 is good just read measures from drawing

G71 type2 i knew, but really make it work lately.

it was pain in ass change parameters.(well not hard but how find what to change)

i dont use G41/g42 on lathe i calculate nose radius compensation for tool path.

no cam needed for it.

rouching cycle not use compensation i read bout it.

so it means rouching cycle should be counted on that

like manual says

i like use same path unless i need control how i finish it.

G73 is good if want do it fast and start cut, but yes its doing lotsa air time.

option is make custom makro G71/G73 variant no air cutting

its like what CAM would do. i have path cut it like this way make it bigger

until reach final. its simple 🙂

i know how make tool path faster than CAM we try it. boss decide CAM not needed.

becouse i am CAM haha.we have 1 program that is popular our country

it is easy to use can get tool path for harder part,but its only that tool path i take

i never make full program send to machine click start.

yes i won cam battle i get part done faster than cam guy post process it.

then change all cutting parameters match. my hand written code run part faster.

reason was i used my own made makros(no need cam if allready know how do it FASTER :))))

you could imagine my boss face

second problem is we are small company and im onlyone could use CAM

programs need be easy to read and short so other can make changes

fusion360 i ty my best for it.simple cut and i never did pass post process allready red red warnings.

there is too many retrack line and other things. my mind i only need countour to cut R plane and blank.

why it need how far i need cut. i just told cut this figure lol. default should be normal G71 style. no way to get collision on simulation. then can enhance it,but fusion360 try do it opposide its try do it best way and cut inside part

i dont get that.WHY its cutting inside part. i have countour i want cut and blank. why its going inside.

if i not learn fusion360 them my fellow worker never learn it

i know i can save my cycle for future purpose, 

G71 cycle is so easy. cut this depth long as you need leave W if added.

retrack 45 degree back with given R value return Z starting point.

start new depth.

last cut final figure leave U and W if given.

i think fusion360 is awesome software for creating complex parts and easy change, but simulating and post processing is pain.

becouse it not simulate it correct it cut inside part.(i not get that)

well never do post process. my head blow off on simulating simple shank lol

[scottmoyse]

why are you commenting on a CAM thread when you don't use and don't want to use CAM?

Kind Regards
Scott Moyse
Manufacturing Technical Specialist Autodesk Expert Elite
P: +64 9 302 4028 M: +64 21 055 7775
[email protected]

CADPRO Systems Ltd
Auckland - 527b Rosebank Road, Avondale Auckland
Christchurch - Unit 3, Kendal Avenue, Burnside
New Zealand

[andrew.todd1]

Hi Akash. any movement on this?

[akash.kamoolkar]

@andrew.todd1 we're continuing to test and fine tune G71, G72 roughing canned cycle output. Just to give you a peek inside the sausage factory, projects like this have a longer development cycle because they involve considerable coordination across several Fusion teams (user interface, kernel, post engine, post processors, QA). We want to make sure we release a feature that works off the shelf so we're doing our due diligence in that respect. But we're getting there.

Regards,

Akash Kamoolkar

[andrew.todd1]

Thanks Akash. Waiting patiently! 🙂

[Anonymous]

Any new word on the can cycle timeline?

Or perhaps anyone know of an add-in that will create a G71 / G72 cycle?

Thanks all.