Modelling a P3 Polygon Profile

[AlanMueller]

I am trying to model a P3 polygon profile for a connection interface (for those familiar with manufacturing, think a Capto shank). This profile is described in ISO 26623-1:2008 as follows:

For my specific polygon:

Dm = 28 mm

e = 0.9 mm

I am trying to draw a sketch and then extrude this profile as a cut with the proper taper as a draft angle, though I may end up drawing the smaller end and using loft.

Any help would be much appreciated! Thanks!

[a.laasW8M6T · Accepted solution]

Hi

Do you actually NEED to model it in Fusion?

You can just download a C4 Blank from a tooling supplier like Iscar, and then do additional modelling if you are trying to create a custom toolholder

https://www.iscar.com/eCatalog/Item.aspx?cat=4510113&fnum=2581&mapp=IT&app=154&GFSTYP=M&isoD=1 

I don't think its possible to do describe curve like that In Fusion but someone more experienced in design can comment on the feasibility of doing this.

Inventor can describe curve with an equation

https://help.autodesk.com/view/INVNTOR/2024/ENU/?guid=GUID-9527E927-0001-4A8F-822E-9A30064B6A8F 

[Drewpan · Accepted solution]

Hi,

I don't think fusion can describe curves with a formula either, however I do think there is a way you can quickly and

easily import the shape for extrusion.

There are software tools on the net that will create the shape from the formula that you can then save as an svg file.

You can then import the svg and extrude from that. Depending upon what precision you need you should be able to

scale the svg to the size you want. If you need great accuracy then you might have to do the suggested Inventor

method from the previous post.

To the Devs

I have also wondered if there is a function in fusion where I can simply punch in a formula and a range of values to

get a 2D or 3D curve. If there isn't then I think that there is enough users who would use it. There are several tools

available from the fusion app store for creating airfoils which are are using this method of formula to curve. There are

also many engineering formulas for creating shapes and parts that a tool like this could be well worth the trouble of

coding and coding it should be straight forward. You already have formulas for simple 2D curves and 3D shapes like

spheres, complex shapes are just different mathematical formulas. The formula for a simple sin wave y = sin A is not

rocket surgery, nor is the formula for a parabola y = x^2. 3D shapes are only one step more complex, a sphere is

x^2 + y^2 + z^2 = A. There is nothing really hard about this, most of the code is already in fusion, all you need is a

data input standard and bingo - it is a new fusion function.

Cheers

Andrew

[AlanMueller]

You guys both had great ideas, thanks a lot!

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@Drewpan  wrote:

There are software tools on the net that will create the shape from the formula that you can then save as an svg file. You can then import the svg and extrude from that. Depending upon what precision you need you should be able to scale the svg to the size you want. If you need great accuracy then you might have to do the suggested Inventor method from the previous post.

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This is an interesting one I didn't consider at all. As you noted, the accuracy wasn't near what I needed, but it did work; I used Desmos graphing calculator  to graph the polar version of the function: (Note I had to swap "c" for "e" because e returned a constant; I couldn't use a slider value. By the way, this function and other modified functions came from a paper I found discussing these polygons: see here).

Then I exported it using the "Share Graph" button and Export Image as SVG, then imported it to Fusion as a Sketch to be extruded. The problem was the SVG came in as pretty long linear segments. So I had to fall back on using inventor.

Thanks @a.laasW8M6T for linking to the instruction on how to create a equation curve. In Inventor, I used these following equations from the same paper mentioned earlier to create a 2D equation driven curve in parametric cartesian mode:

x(t): (( Dm / 2 ul ) - e * cos(1 deg * 3 ul * t)) * cos(t) - 3 ul * e * sin(1 deg * 3 ul * t) * sin(1deg * t)

y(t): (( Dm / 2 ul ) - e * cos(1 deg * 3 ul * t)) * sin(t) + 3 ul * e * sin(1 deg * 3 ul * t) * cos(1deg * t)

I was able to export the sketch as a dxf and import into Fusion for extrusion. I used Flex tokens to access Inventor; $24 is a bit steep for a single curve, so I exported curves for each PSC variant. They are attached below, along with my Inventor part file, if anyone would like to use them.

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@a.laasW8M6T  wrote:

Do you actually NEED to model it in Fusion?

You can just download a C4 Blank from a tooling supplier like Iscar, and then do additional modelling if you are trying to create a custom toolholder

---

I need a female version of the interface. So potentially, if I was good at surface modelling, I could've found the curve that lay at the intersection of the tapered surface and flange surface, which would have maybe been the nominal curve, then re-extruded it to get the receiver form. The receivers have a slightly different taper to them (Shank: 1° 26' 21"; Reciever: 1° 25' 31") so the actual surface of the tool shank model provided by Iscar or other manufacturers wouldn't match the receiver surface.

Thank you both for your ideas!