knurling on tapering cylinder

[m.rittweger]

Hi, all!

I need to put a knurling on a tapering cylindrical face. I can't just use a texture, because it will be 3d printed.

The details: I have a cylinder with a diameter of 60mm and 10mm height. Then there is a cylindrical shaft from 61 to 51mm with a height of 119mm on top of that. And then there is a cylinder with 50mm diameter and 10mm height. Finally there is a centered hole with 12,5mm diameter from top to bottom.

I was able to design a shaft with 50mm, 51mm and 50mm and a knurling on top of the middle shaft. Of course that was no problem with 60, 61 and 60mm, too. (see picture below)

( Yeah, I know, it's hard and time consuming to render that knurling. But hey... 😉 )

With the tapering surface I have the problem that the helix doesn't follow the surface, but ends up in mid air (see picture).

So how can I achieve this?

Michael

[jhackney1972 · Accepted solution]

Are you trying to use a Coil to create your helix cut or a Surface Sweep?  The Coil command has a taper feature if that is what you are using.  Attached both your cylindrical and taper knurl (attempted) so we can see what you are using.

[Drewpan]

Hi,

Knurling is usually done with a tool on the machine you are using to turn the workpiece. It is going to

be a bit different when you 3D print.

I would suggest to simply create one small square pyramid at the start point of the knurled feature, and then

create a round or square pattern of these shapes on the surface of the body. If necessary, select all and join

them to a single body and bingo - knurling.

The knurled feature also doesn't have to be square - as long as it creates the texture you want for the knurl.

I have seen small circles, interlocking triangles, hexagons - whatever.

Fusion doesn't handle knurling well, mainly because all that detail is a nightmare to model and it slows down

processing because of that same detail. Typically you would model it like a thread - show it but don't actually

cut the thread on the model, modify the CNC code to make the cut on the workpiece.

Cheers

Andrew

[m.rittweger]

Hi, John!

Thanks for your answer. In fact, I did tinker with the "degree" of the helix. It was a bit tedious, because I had to trial and error with the underlying cylinder for that value. In the end it was -2.4059 degrees. While that value in the helix didn't work I seem to have forgotten it after some time.

The helix cuts at the start into the cylinder but doesn't follow the surface and thus the engraving get tinier and tinier. See picture below, engraving only in the lower part.

BTW: Is there a simpler solution to define the tapering? The start at 61mm and the end at 51mm is fixed. Actually I need 119mm in height. That produces those -2.4059 degrees after trying a bit, a bit less, using the next decimal etc. At least the result was a 51.00mm diameter shown in the upper sketch. Horrible thinking of changing the height to, let's say, 139mm.

Michael

[m.rittweger]

Hi, Andrew!

Yep, I've done knurling on a machine. Roughly some 40 years ago, no CNC then... 😉

I think your suggested method is quite like the (various) hints and tutorials found in the net.

(very rough)

A rhombus at the base edge

A helix with outer diameter

A second helix with outer diameter + 4

A cutting sweep with the rhombus along the helix

A mirror of the sweep

A round arrange of the sweeps

And yes, it takes a tremendous amount of time to render, at least with my actual 119mm height, 1.5 turns, mirror and 45 times arranged. Unf. I can not modify the CNC code afterwards. I will export an STL or 3MF to the slicer that cuts the model in horizontal layers and send it to the printer. Thus, like a thread, it has to be modelled in Fusion, not only shown.

Michael

[Drewpan]

Hi,

That is the difference between modelling and making. As I said, normally we would make it look like it was

knurled and tell the machine to knurl it. Because you are 3D printing it you actually have to model it.

I am just wondering if you might be overthinking it a bit.

Try to simply model a single shape, then use the line tool to fit them in to a single line, then rotate that

whole line around the barrel of the shape. Saves helixes and mucking about. I suppose it comes down to

how much definition you want it is "just a knurl" after all. A 3D printer will print what you tell it to.

You could always "cheat" and print it smooth then pop it into the lathe and use the knurling tool? It

is only plastic so it should work.

Andrew

[etfrench]

Here's one done with your calculations.  I added 5mm to the top and bottom of the coil in order for the coil to extend through the top and bottom.  The size at the bottom of the coil was calculated in a formula in Sketch4.  The parameters of the coil can be edited in the Parameters dialog.   I don't really like 60 degree knurls, 120 degrees would be best visually.   It might be better to create the helix in the surface workspace (just a sweep with twist) and use that to cut the face of the cone which would then be used to sweep the desired profile.

[Warmingup1953]

Just a quick "play" before heading home::

Using Sheetmetal and Unfold. I know this approach can't "meet Up" but as I said just a play whilst I ponder further over the Weekend.

[TheCADWhisperer]

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@m.rittweger wrote:

I had to trial and error

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@m.rittweger 

You don't have to use trial and error.

You can set up Parameters that automatically update.

I didn't take the time with this example, but it it easy to set up parametric trig equations.

BTW -  you keep stating "cylinder" but then describe what is called a "cone" in geometry.

[m.rittweger]

Hi, Andrew!

> Try to simply model a single shape, then ...

I'm not sure if I understand what you mean resp. what I have to do. 😉

In SketchUp it is a bit easier: Draw a circle, extrude in height and scale the upper circle. So I don't have to hazzle about the degrees. On the other hand... that helix thingie is a pain in SketchUp. It is very, very hard work to model a thread or the like.

> ... print it smooth then pop it into the lathe ...

Well, I don't have a lathe. 😉 I just learned a job dealing with metal that roughly 40 years ago. I soon switched over into the IT direction. Now I'm a business analyst. 😉 Our company produces and sells large diesel engines (for cruisers etc.), though.

It won't help knurling the part after the print. The print is kind of hollow and has only a few walls around the infill. See the complete grip as exported from Fusion360 to the slicer (OrcaSlicer in this case) in the picture below. And the 2nd picture shows the sliced model in roughly half way in height. You can see the outer walls (3 times 0,4mm) and the infill. With 1.2mm outer wall and a 2mm knurling that would... uhm... well... 😉

(Yep, it's not the exact model I'm working on right now. This one hasn't the hole in the center.)

Michael

[m.rittweger]

Hi, etfrench!

> Here's one done with your calculations.

I tried to remember a bit from Pythagoras and ended with a model seen in the picture below. It validates my 2.4059 degrees "trial and error" 😉 (at least right after I remembered that " * 180 / pi " clause...)

Now I'd love to make up the whole thing with parameters. I still have to figure those ones out, methinks. 😉

Actually I have some measures derived from other ones. Like: The rhombus at the base (for the cut out) has a measure of 1/3 of another measure (see below). But that's not "parameter" I'd guess.

I'd try to

- set the "turns" of the helix at 0.5 per 100mm, thus right now it's at "119 / 100 * 0.5". This is written as exactly this in the "turns" field of the helix. Now it would be nice to see a "height / 100 * 0.5" there. But I don't know where to get "height" then. (Later on I might try 0.75 turns per 66mm or whatever.)

- set the "amount" in the circular repeats to "diameter - 10%". So right now with 51mm I have set it to 45. Would be nice to play around with other values for that, too. Maybe dependant on the depth of the engraving, too.

> ... create the helix in the surface workspace (just a sweep with twist) and use that to cut the face of the cone ...

I'm not sure, but I think that's exactly what I did (see below).

Thank you very much for the f3d file. I will have a look into it asap.

Michael

[m.rittweger]

Hi, CADWhisperer!

> You can set up Parameters that automatically update.
> ... it it easy to set up parametric trig equations.

Just see my answer to etfrench. Yep, I realized a model around the 90° triangle. So as

alpha = arcsin ( a / c ) * 180 / pi

where

c = sqrt ( a² + b² )

a = ( lowdia - uppdia ) / 2

b = height

So this has to be set up as parameters for lowdia, uppdia and height. 😉 I'll figure that out... sooner or later... 😉

> you keep stating "cylinder" but then describe what is called a "cone" in geometry.

Yes, you're absolutely right, thanks. That word slipped out of my mind.

And thank you the the f3d file. I'll have a look into it asap.

Michael

[Warmingup1953]

Eventually, I got close to what I was trying to achieve but boy did it tax the PC resources!

[m.rittweger]

Hi, all!

I still don't know where my mistake sits. The "cut" helix (red) doesn't follow the "rail" helix (blue) as seen in the picture below. Instead it drifts away from the cone as if it were a cylinder.

Still maybe another problem: The rail doesn't start at the cut position, but 180° opposite. 'With a cylinder that wasn't a problem, but with the cone it might be? Not sure...

Michael

[TheCADWhisperer]

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@m.rittweger wrote:

Hi, all!

I still don't know where my mistake sits. 

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@m.rittweger 

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[m.rittweger]

Hi, CADWhisperer!

> Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

I could, but maybe it's not needed anymore. 😉

I started a new component from scratch and that one does not show any of the above mentioned problems.

I made the following steps, as shown in the pictures below. My last question at this point would be: Is this a correct way to achieve it? Or is it absolutely nonsense and I should use another way?

Thanks for all your support, to you all!

( not sure, which answer I should mark as answer, but the "degrees" answer by John and/or the "parameters" answer by you. )

Michael

sketch 1

 

 

extrusion 1

 

sketch 2

 

 

coil 1

 

coil 2

 

sweeping 1

 

mirror 1

 

circular 1

 

extrusion 2

 

the final model

 

[etfrench]

Open the parameters dialog in the file and adjust the values until you get the desired results.

[m.rittweger]

I played a bit with the parameters now. I renamed all used parameters to meaningful names. Ok, I renamed the (more or less) unused parameters, too. 😉

I can change "test_base_dia" to 61, "test_base_height" to 119 and "test_top_dia_bore" to 12.5 and get a result that looks not too bad.

My problem was using e.g. the value for ""Revolutions" aka "test_coil1_turns". I wanted to use "test_base_height / 100 * 0.5", but F360 rejected this with an error. I solved it, but am not sure if I used the correct way: I have set "test_base_height / mm / 100 * 0.5" --> The test_base_height has the unit [mm] while test_coil1_turns has no unit. So I thought it would be a good idea to shorten "* mm" by "/mm". Or is there another way?

Now my last problem actually is the test_base_angle. That's where I have to implement the Pythagoras model and I don't have a clue how I can do that. But I'm working on it. 😉

 

Michael

[TheCADWhisperer]

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@m.rittweger wrote:

I don't have a clue how I can do that.

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@m.rittweger 

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[m.rittweger]

Hi, CADWhisperer!

I tried a lot and finally got a more or less working model with parameters.

My problem was the syntax of clauses within the formula. I was'n able to just use "test_base_dia" but I had to use "( ( test_base_dia / mm ) * 1 deg )". This made it a bit difficult to get the formula up. But in the end:

 

-asin(( ( ( ( test_base_dia / mm ) * 1 deg ) - ( ( test_top_dia / mm ) * 1 deg ) ) / 2 ) / sqrt(( ( ( ( test_base_dia / mm ) * 1 deg ) - ( ( test_top_dia / mm ) * 1 deg ) ) / 2 ) ^ 2 + ( ( test_base_height / mm ) * 1 deg ) ^ 2))

(A) and (C) can be set freely to any value. I had a bit difficulties with (B). Only a "driven measure" (correct translation?) within sketch 2 showed me the 51mm. Now I added a circle into sketch 1 to get that variable, too. 😉

Now my (last? 😉 ) question: Is it possible to change the 3 parameters in the rendered model view already? Or does one have to go to the "change parameters" dialogue?

Michael