Community
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.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Thread on face of part

26 REPLIES 26
SOLVED
Reply
Message 1 of 27
andrew.todd1
820 Views, 26 Replies

Thread on face of part

Hi guys

 

See attached pic. Im trying to machine a spiral groove on the face of a turned part. Can this be done in Fusion?

 

Any help welcome.

 

Thanks.

 

Capture.PNG

 

 

26 REPLIES 26
Message 2 of 27
VicKosta
in reply to: andrew.todd1

In the past, I used threading cycle to create texture on part face that increased bonding surface for glue application.

Simply typing in few passes using G32 did the job, In Fusion I can only select ID or OD but not part face, so it looks like answer is NO.

Message 3 of 27
seth.madore
in reply to: andrew.todd1

Using the Spiral command, you should be able to accomplish what you are looking for. You likely won't have the option of Start point, but it should get the job done. Set inner and outer radius size (don't forget to add or subtract your tool radius), set your Stepover and you should be pretty much in business 🙂


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 4 of 27
andrew.todd1
in reply to: seth.madore

Hi Seth

 

is this a turning operation?

 

Cant seem to find 'spiral'?

 

Fusion file attached if you can point me in the right direction.

 

Thanks.

 

 

Message 5 of 27
seth.madore
in reply to: andrew.todd1

Ohhhh, my apologies. I didn't see the mention of "turned". No, Spiral would not work, as that's a milling toolpath.

Do you have a certain pitch to hold? I'd imagine just using a turning path with a coarse feed would get you what you need, although I don't know if that would give you a synchronized infeed. I think you are back to where @VicKosta  pointed you


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 6 of 27
VicKosta
in reply to: andrew.todd1

I got "Thread on face of part"  as being related to ..... threading, .... so no option in turning, spiral is milling strategy.

Manual programming using G32 should work.

Message 7 of 27
VicKosta
in reply to: VicKosta

G32 is used in tapping cycle, it clamps feed rate to given pitch so that you cannot change it by moving manual feed rate override button away form 100% which would cause tap to break.

I once asked a supervisor on my new job why they use G1 for tapping, he sarcastically answered, "because it works" and I had no heart to burst his bubble by "accidentally" altering feed rate button position, it would be bad impression on my first day,  following instructions and working with other people, especially with questioning "authority".

 

So, you want to create few loops, starting above top diameter and exiting below small diameter.

Rapid in position above large diameter and  .1 from face, on next block rapid in Z minus position for first pass, feed down in X axis past stock using G32 and whatever pitch you require for feed rate.

Rapid out to start point in Z and then above large diameter.

Repeat this 4 moves loop as many times as number of passes you wish to take, increasing Z depth on each pass as you progress.

If taking 10 passes, decrease depth for each pass to keep chip load proportional.

 

G32 will also enable encoder to keep tool in sink with spindle and start each pass from same point so as to not cross thread the previous pass.

Using G99 (feed rate per revolution), you can also use G96 to control constant surface speed and achieve uniform finish between two diameters.

 

(20 TPI)

T0101

G50 S1000

G96 S300 M3

GO G54 X4. Z.1

M8

Z-.01

G32 X2. F.05

GOZ.1

X4.

Z-.014

G32 X2. F.05

G0 Z.1

X4.

Z-.016

G32 X2. F.05

G0 Z.1

X4.

Z-.0175

(ETC)

 

 

Message 8 of 27
andrew.todd1
in reply to: VicKosta

Thanks for your help on this. It looks like I gotta look outside Fusion for this one and it looks like your pointer is my best option Vic.

 

I'm guessing if I need to change the 'pitch' I need to adjust the F value? im looking for 40 tpi.

Message 9 of 27
VicKosta
in reply to: andrew.todd1

Yes, for 40 tpi your feed rate will be F0.025 / rev. I am not sure what exactly this is for but the concept is there, just adopt dimensions to your need.

Also, careful with RPM's, if your machine fails to wait between passes until speed is adjusted before each pass, just use G97 instead of G96 or use dwell before each pass.

Message 10 of 27
andrew.todd1
in reply to: VicKosta

see pic. this is what im trying to acheiveCapture.PNG

Message 11 of 27
VicKosta
in reply to: andrew.todd1

Well, that changes the whole ball game, you started with post about thread but your print calls for grooves of pitch density between 24 and 40 grooves per inch.

I think threading is not the answer here, what profile is the grove?, is there a sectional view shoving radius or "V" type of groove.

I think you just need to write a G-code to turn groves at desired pitch of about 32 / inch, can be G74 cycle, long hand or model the grooves and have Fusion take a crack at them if that is your preference.

Judging from surface finish requirements, I'd guess this is just bonding surface for rubber or plastic element, wish you posted that earlier.

Message 12 of 27
andrew.todd1
in reply to: VicKosta

See attached. This is really ALL the info I have and the customer isnt very helpful.

 

would you be able to help with the g code option? Unless fusion can do this?

 

Capture.PNGCapture1.PNG

Message 13 of 27
andrew.todd1
in reply to: andrew.todd1

also, some feedback i got on facebook..

 

Capture.PNG

 

 

Message 14 of 27
VicKosta
in reply to: andrew.todd1

I assume note pointing to part face supersedes one on lower left corner, if your customer is not helpful in defining what needs to be done, I don't know what they want either.

First thing is to determine what EXACTLY needs to be done than find a technique to get it done.

 

"Series of concentric grooves" or "spiral grooves" , have to know what customer wants to know what to do.

Message 15 of 27
andrew.todd1
in reply to: VicKosta

Its a spiral on the face shown. Apparently its very common in some circles. See below. will this machine a spiral?

 

N3
(FACE GROOVE TOOL)
(SERRATED SPIRAL GROOVE)
G0 G20 G40 G80
G50 S1000
G96 S300 T0505 M3
G0 X1.8 Z0.1 M8
Z-0.025
G32 X0.7 F0.025
G0 Z0.1
X1.8
Z-0.05
G32 X0.7 F0.025
G0 Z0.1
X1.8
Z-0.075
G32 X0.7 F0.025
G0 Z0.1
X1.8
Z-0.1
G32 X0.7 F0.025
G0 Z0.1
X0.950
G0 G28 U0. W0. M9
M5
M30
%

Message 16 of 27
VicKosta
in reply to: andrew.todd1

OK, look back at my post  (7 of 15), I gave you identical G code pattern  and asked you to adapt the concept to your need, your need before I ever saw print in upper post.

Yes, this and my posted code will cut spiral groove or "thread" on part face. The depth and pitch is determined by Z coordinates and feed rate / rev.

125 - 500 surface finish would suggest that only one .001 - .002 deep pass is enough to generate required texture, just an estimate.

Use threading insert for 40 tpi, having very small radius on tip, make one or two passes using F.025 .

You would then compare resulting finish to "Surface roughness Gage" for turned surfaces, or measure it by instrument called Profilometer (spelling ??).

 

Looking back at your print and circled note I see "SERRATED SPIRAL GROOVES" , so it is fair to say that threading pass will be compatible with requirement.

If in doubt about result, consult with customer, perhaps there is a sample part they can provide.

 

If you Google "Haas programming manual", handful of ".pdf" files pops up, free download, plenty of G code wisdom in any of them.

I cannot comprehend anyone attempting to do complex machine work without having fundamental knowledge of programming and hoping to get all answers in internet forum.

 

My employer has no idea how to do things I do, that's why he hired me, I get compensated for analyzing prints, planning processes, programming and making parts, I use handful of other tools besides Fusion and I am in trade for 35 years and counting.

I started by reading machine manuals and analyzing NC programs I found  in control of first CNC machine I ever touched.

 

Message 17 of 27
andrew.todd1
in reply to: VicKosta

At what stage did I give you the impression I dont have a 'fundamental knowledge of programming'? It it unwise to be

presumptuous my friend.

Message 18 of 27
zwelsh91
in reply to: andrew.todd1

I am truly intrigued by this thread, seeing as I have never encountered a print call-out for a surface finish such as this.

From all of the info posted above and the sample code you have I would think you could produce satisfactory results purely based on the code itself that you have posted, but in the physical world that is another story. I wish I had some experience with this sort of thing and could be of more help. Do you have a way to test your code (on a test piece of material)  so that you can "Prove Out" the process? I would be inclined to run a test just to prove to myself that it would work.

Zak Welsh
Zakary Welsh Machine LLC
Message 19 of 27
seth.madore
in reply to: zwelsh91

Vic did provide the correct answer and reasoning. It's typically required for gaskets and adhesives. A threading toolpath aligned with the X axis "should" do the trick. Choice of tooling/inserts is usually determined by customer. I've seen them done with small radius P.H. Horn tools, custom wired form tools, you name it. 


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 20 of 27
VicKosta
in reply to: andrew.todd1

Well, you got all the right answers and yet you did not connect the dots, such as comparing my suggested G code to one you got from Facebook, I had to point it out when you asked if one you got from Facebook will cut thread on part face.

That really sounded an alarm here because it doesn't look like you overlooked it, in thread you started with limited information, it looked more like you had no clue as to what you are looking at.

So, my friend, for your safety, I sure hope you "speak" G-code and are not relying on Fusion to produce one that may or may not blow the door off of your lathe.

 

This one missed me by inches, someone cut the cycle time by wide margin, efficiency before safety, ..... ISO certified,

one of those....."leading manufacturers".

Cheers !

 

1348113320514.jpg

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

Post to forums  

Autodesk Design & Make Report