Knurling on a curved surface

[Anonymous]

I am  trying to make a knob with knurls on it. I can do it on a flat knob but not on a knob that is curved.

Screenshot 1 is knurls on a flat surface, I can do it fine, what I need is basically the same thing but on a curved surface.

Screenshot 2 and 3 is where I can get to before I get an error for the circular pattern if I choose the number of repeats I need. I need the knurls to line up perfectly along the curved surface like how they are in screenshot 1.

[Anonymous]

Attached is my file.

[mcgyvr]

Besides ensuring all sketches are fully constrained

If you press the >> button in the lower right of the pattern dialog box and select "adjust" for the creation method you will have better luck.

The "to next" extrusion needs to adapt for each instance of that pattern and "identical" does not allow that to happen..

[Anonymous]

Thank you for the reply I fixed the sketches and changed the pattern to adjust. Now I need to get the patter to wrap all around the circle, but if I pattern it around the circle I get an error. 

[mcgyvr]

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@Anonymous wrote:

Thank you for the reply I fixed the sketches and changed the pattern to adjust. Now I need to get the patter to wrap all around the circle, but if I pattern it around the circle I get an error. 

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Ok.. Either adjust your original sketch to have Revolution1 centered around the X origin axis so you can use that or create a new axis on in the center of that Revolution1 using the Axis "Through Revolved Face or Feature" function. 

[mcgyvr]

Oh and expect to bring Inventor to its knees as its not really capable of handing such geometry without a massive performance hit..

Hopefully you just need to do this once to 3d print the part and don't it day in day out.. 

[cadman777]

Have you tried adding a raised face to the existing surface and making a cut in the raised face instead, and then patterning it? I believe that's how a knurl is made. But like mcgyver said, you're asking the software to force the computer processor to get hung up on your knurl. WAY too much overhead. It's like making fully formed threads (spiral triangles) on every fastener in your model!).

[johnsonshiue]

Hi! This can be done fairly easily. The trick here is how you manage the Boolean operation. If you pattern the extrusion as a feature, the faces and the individual feature has to be replicated many times. For a curvy part like this, you can end up with near tangent conditions and the Boolean may fail.

Instead of patterning the features, you can pattern the body. I make the Extrusion a bit bigger. And, pattern the body as joined body. The combine the knurling body with the base. The result is much nicer and the compute is much faster.

Please take a look at the attached part.

Many thanks!

[andrewdroth · Accepted solution]

Here's my attempt.

I had to take some liberty with the tool path and tool, but I think a sweep-cut with a twist sort of works.

It makes for a very feature heavy part though. I don't know if Inventor would handle a full rotation of these features.

[cadman777]

Yup, that's what I was talking about, agreeing it would take a miracle to make the knurl uniform across the bend (it's not a true knurl!). And yes, it's very 'heavy' on the resources, which is why I never make these kinds of features unless that's all I'm detailing on a part (which is rare to never).

Glad you made it work!

[Anonymous]

this seems pretty close to what I am looking for but I am using Inventor 2018 so i can't open the file. How do you do the sweep? do you project a line to the surface and draw a triangle for the cut on the edge? Thank you.

[andrewdroth]

Yes, that's exactly what I did. The starting position and twist angle were also critical.

Ideally the sweep profile would match the outer surface perfectly, but for whatever reason the sweep would not compute using a 'projected cut edge' or a 3D sketch 'project to face' curve. So I just approximated the shape using one arc. That is why the tips of the knurling vary in size though. You could probably use a spline or multiple arcs to get a better approximation.

The cutter needed to be tilted relative to the path at the start, and rotate (twist) along the path to look right. Since my path was cut at 45 degrees to the center line I used 45 degree tilt for the profile and a 90 degree twist for the sweep. It seemed to work out well, but I don't know if those angles correlate exactly.

Let me know if that makes sense...

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[andrewdroth]

I lost the screencast there, I think?

[cadman777]

Nice!

Did you try creating the cutting profile at top dead center on the curve?

To get the exact profile, you can create a work plane on the 45° line, and then do a 3d intersection of that work plane and the object's surface. Then sweep the cutting profile from t.d.c. along that curve.

[Anonymous]

Yeah... putting the profile at the center would have been better. Not sure why I didn't think of that.

Like I said, the sweep wouldn't compute on the projected curve. I could select it, it just wouldn't preview.

[andrewdroth]

^^^ wrong account, same guy.

[S_May]

@Anonymous 

here is a pattern..... 🙂

[johnsonshiue]

Hi Guys,

Here is the modified version of Andrew's solution. The Sweep was created as a new body. Then it was patterned and mirrored as a body joined together. The part has EOP rolled to the top because it is a giant 250MB part. You need to move EOP to the bottom. It may take a while due to massive amount of geometry.

Many thanks!

[Anonymous]

I got Inventor 2020 and was able to open the file and yours is working great, exactly what I needed. The only problem I am having is the mirror feature, it is coming up 1 short of what I need and I am not sure why, I attached the file if you could check it out that would be great, thanks!

[andrewdroth]

I think you just need to add Sweep4 to the mirror just selecting the pattern excludes it.