cutting spiral grooves

[slaughlin79]

i am able to get all the machine work at my job and that work involves cutting a spiral groove in the face of a part front and back just like the grooves found on a pipe flange. to be exact the part will be sandwiched between two flanges.  ive got everything else figured out but i cant find a way to make the cuts. i planned on turning the part in my 4th and have my spindle come down and touch off with a single form thread mill and cut the phonographic groove but i cant find an operation that will allow me to follow the projected path and while using a form mill. attached below is a test model and maybe someone can tell me if its possible or not?  

[Anonymous]

You cannot use 4th axis to cut continuous spiral because it requires wrapping tool path around cylinder in order to drive 4th axis but wrap only works on single diameter.

If  you are bent on doing 4th, instead of having spiral geometry, make concentric circles and produce individual 2D contour wrapped tool path for each groove, each time offsetting wrap diameter for difference between circles.

It can be done but cutter geometry and orientation will be in conflict with grooves at some point after very shallow pass.

Use engraving tool instead, if material is steel, make few axial passes. I've done something like this many years ago on lathe, using threading cycle and single point threading insert, texture was used for application of glue.

[engineguy]

@slaughlin79 

Personally I would just do it in a normal 3 axis setup, simple Trace toolpath using the Axial offset to get your desired depth and a V pointed tool (Chamfer Tool) for the job.

File attached.

Stay Safe

Regards

Rob

[Anonymous]

😋🙄

[slaughlin79]

I wish I could do it without the 4th and one side could absolutely be done that way but the one side has a cone shape that starts out small at the flange and gets bigger as it moves away from it. It would take an over extended and very slim took holder but still Even then I don't think it would clear the top of the cone part of body. I will post that actual drawing when I get my laptop from home and you will see what I'm talking about. I did notice that It would do a full circle and I could step down multiple time like Vic said. That might be the only realistic option. One way or another i gotta figure a way to do it.

 It's hard to imagineto think that as complicated as 5 axis toolpatha are and how well fusion does them that 4th is lacking so much. Not saying it's useless bc it still does some amazing things but don't call it 4 axis when it won't use all 4 axis' simultaneous. 

[seth.madore]

Nope, totally agree. They went from great 3 axis to decent 5 axis, but rather skipped over the needs of the 4 axis guys 

I have a 4 axis mill in my shop 😉

[slaughlin79]

i wonder why that is that they did it? fusion 360 its so close to be the perfect cad cam software and im sure is for some but i just wish they would show equal intrest in all 3 being 3,4 and 5 axis. but anyway heres an unfinished model but yall will see what im needing to do.

[seth.madore]

I think it's a market share thing. A lot of shop jump from 3 axis to 5 axis. And for those with 4th axis abilities, it's MOSTLY just 3+1 positioning and machining. The roots of Fusion CAM are steeped in metal working, so things like billiard cue turning or  other types of 4 axis milling never rose to priority

[Anonymous]

After some pushing and pulling, closest I can get is this.

[Anonymous · Accepted solution]

Weird stuff, only way I can do back side is by using circular pattern.

I tried duplicating tool path and selecting contour on back side but error pops up.... "No contours have been selected"

At this point, if serations have to cover entire face, I would adjust front inner height, produce G-code, than adjust inner height for back side, post and delete front side from it then combine resulting code.

[slaughlin79]

i wonder if another another cam software can do it? im only firmiliar with fusion so not sure. i wish i was but im not comfortable enough to start modifying posts.

[slaughlin79]

VicKosta BRILLIANT! thats what i was needing. thank you so much! now i gotta figure out how you did it. ive tried using pattern before and i couldnt figure it out but i didnt put much time into it. i will certainly dig deeper now. i just got a vf4ss and it took way more than i had and thinking i was going to need to buy a lathe or very expensive software which i absolutely cant do, you might have saved my ass. fingers crossed man

[Anonymous]

So, my focus was only on one objective, ....... "how would I do this if I had to". It's not in line with my earlier proposal but that's why it takes experimenting to come up with something.

Tool size and other values are totally random so you'll need to adopt things to actual tool and print requirements.

I'll give you few hints, sketch driving tool is on offset plane .01 below model top, circle has .001 wide break to allow unwrapping and after not being able to duplicate tool path for back side, I added sketch line in the middle between front and back then used it as axis for circular pattern rotation.

I realize concentric circles are not the same as spiral but I see no other way unless you manually code it to drive A axis 360 degrees multiplied by number of winds, while driving Z axis from start to finish of a spiral at desired  pitch.

I have done similar job on a mill-turn few years back, cutting  spiral groove on OD of a part by incrementally rotating C axis 5 and a half turns and simultaneously driving Z axis required distance for each revolution of C axis.

[slaughlin79]

Sorry, I forgot to except solution days ago. But I was gonna come back and give an update. You absolutely 100 percent saved my ass. I looked at how you set everything up and looked a sketched and it started making sense fast and Extrememly relieved and happy to say I got operations applied two all 4 sizes of the parts I will be machining and also did a text cut in a piece of aluminum round stock and it's perfect. Used a 3/4 single form 60 degree thread mill, .04 or 03 step down and on stock to leave I went with -.018 and it looks and even feels better than the grooves that were made by the shop that is machining then now on a lathe. Couldn't ask for better results. One more time,thank you so much and all the other members that take the time to not just help someone but to go into detail and help someone.

[slaughlin79]

spiral grooves are not really what you want. Complete closed off, concentric circles is what is preferred but most flanges and grooves are made on lathes and it's just way easier to spiral a cut as I'm sure you know so the way you showed me is a better solution than what I was going for. Had to throw that out there.

[TomD]

I know that this is a Fusion forum and I'm by no means a G-Code guru, but I went through this with "rotary" too for "turning on a mill with 4th" and it seems to me like a 1 liner of G-Code will get spiral stuff like this done and sometimes isn't even worth booting up the software. Position outside the tool at the X cut depth you want G1 Z(finish depth) A(360xnumber of rotations) F(some rate).  Sure you have your moves in/out of the cut to add but thats not overly difficult either. 

If you wanted actual circles you could do it with a subroutine but thats a bit more serious.

I do wish that Fusion made 4th axis stuff more friendly considering the relative ease this should be possible.

ETA I just realized your feed rate isn't optimized through most of this since the diameter is decreasing.  That would be the advantage of the software doing it.  You could do it in stages and change the feed accordingly or pick some middle of the road feed and have worse cycle times.

[slaughlin79]

I just noticed I spelled accept wrong above and had to correct it. I’m not an idiot I promise ha.