IS THERE A SIMPLE EASY WAY ?

[dho]

it will take me to make many planes, extrusions, coils... piece by piece to stitch together, to have an exact slot cut mimic a end mill cutting on the cylindrical body. any easy way?

thanks.

[dan_inv09]

Pi * diameter * angle / 360 degrees will give you lengths for a flat pattern to emboss onto your cylinder, then fillet it.

[JDMather]

Two was that I know.

Technique 1 involves a curve driven patten of extruded (negative) cylinders.

Technique 2 would be an adaptation of this (for your specific problem) - http://home.pct.edu/~jmather/content/DSG322/Inventor%20Tutorials/Inventor%2011%20Tutorial%2011.pdf

Possibly a Technique 3 - Sweep with Guide Surface.

[JDMather]

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@dan_inv09 wrote:

Pi * diameter * angle / 360 degrees will give you lengths for a flat pattern to emboss onto your cylinder, then fillet it.

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Can you post example?

[dan_inv09]

Okay, it won't fillet correctly.

JD, you know I can't post an example because you know that doesn't work, but can you explain why?

The surface method didn't look all that "easy" to begin with and it's looking even harder given the shape at the bottom.

All that constructing and removing etc. and then you end up with planes that intersect or don't ...

And then we should always look back at the original post, it seems to imply that stitching surfaces has been tried already so although we may be able to construct what is shown, the correct answer to "IS THERE A SIMPLE EASY WAY ?" appears to be no.

With the enhancements in the latest release, is it possible to do it with a sweep (or two)?

[dan_inv09]

When did you add 3?

I didn't roll up the eop so I could leave some of the junk that I'd discarded. I can't seem to get rid of the the little ridge!

I didn't use a guide surface - is there something wrong with what mine did (other than the bit I mentioned)?

[JDMather]

Your "solution" would indicate milled with a ball end mill.

From the drawing I interpreted and end mill (no hemispherical bottom the slot).

Did I miss something - or does is this not the exit of the slot indicating end mill rather than ball end mill?

[WHolzwarth]

How about that?

I've included both ways of milling. If you leave EOP above Base1, you'll see flat-bottomed slots.

If you move EOP to the end and switch Solid1 invisible, you see a ball-ended shape, that can be used for substraction. I've only used a radius of 0.0625 in, because the groove is getting flatter at both ends.

Walter

[dho]

Thanks to everyone.

i did it.

[dan_inv09]

You know, I have no idea why I assumed it needed a rounded bottom. That was the only thing giving me trouble - if it has square corners in the bottom then the emboss is probably more than close enough.

So, some follow up questions:

What is wrong with the emboss that it won't fillet?

Why is an offset surface more accurate (or more "square" or more smooth or whatever it is) than the emboss?

And how can we get rid of the little booger where my two sweeps come together (or branch off depending on which direction you're cutting)?

And, what's probably even more important, is there a way in Inventor to detail it? What view will "unroll" it, how do we dimension the angles if we can get it flat?

(Hey, speaking of unrolling - could we have done it in sheet metal? - and how would a sheet metal solution work as a "cam"; I assume your tutorial was made to have a pin or something mate and slide along as it turned - now, were the surfaces needed to work the constraints rather than for accuracy, because for some reason Inventor prefers a surface to a face for a Transitional Constraint?)

[JDMather]

A pin transisitioning in the slot is the same as a cylinder (end mill) that makes the slot.  But it is not as simple as sweeping a rectangle as the tangent point between the cyldrical pin and slot is continuously variable.

https://forum.solidworks.com/thread/78005?tstart=0

I'll try to check the posted solutions and report back.

[dan_inv09]

You could have patterned the emboss rather than making three separate ones.

You could have made holes or cuts instead of "spokes" and combining to remove them.

You could have made the body a revolution instead of a disc and then cutting the bores, or make the bores as concentric holes, or one countersunk hole.

Um... there's probably some other stuff you could do to simplify it, but congratulations on making it work for you.

Roll down the EOP.

Now back to my failed ball mill solution: I don't know if you can see it, but there is a sort of double line along the ridge there

somehow the two sweeps create a funky edge there, could that have been complicating my efforts to remove it?

[dho]

thanks

[dan_inv09]

And every infinitesimal step along the angled path is going to swing it along a little and nibble a little back where it already cut, it's going to be a sort of involute. So you could do a sweep, but the profile really would need to be calculated (and approximated with a spline?) ... when it starts getting that complicated it's time to go back and look at redefining the problem, what do we really need it to do.

[WHolzwarth]

It's no really new problem. In dho's sample with only a small pitch angle, it's not evident, and it doesn't matter, because manufacturing normally doesn't realize that.

But if pitch angle gets steeper, it's getting visible. See my sample.

In the yellowish part an embossed groove is done. The blue part uses the same sketch, but here a middle surface is created first. After that a Both-sides-Thicken operation created the groove.

I've placed a small pin in both grooves. It should have no contact zone at all in the thickened groove, but there's a tiny zone left. I think, I should take a closer look.

But watch the embossed groove. You can see a remarkable intersection between pin and groove.

Conclusion: For working pin-groove combos and steep angles, thickening is needed. Emboss doesn't do a sufficient job there.

Walter

[dan_inv09]

I'm trying to get my head around what you did - the slot runout and the chamfers and stuff are part of something different? And there seems to be some removing then adding back then removing once again?

But the important thing is:

a surface for the center of the slot, thickened both ways - no need to create and delete, and offset, and extrude and extrude and extrude.

I'm in the middle of something so I don't have time but, how close can we get to the Tutorial in the pdf above with this thickened surface (and what's the final difference in number of steps)?

[WHolzwarth]

Hmm. I didn't save my last version to forum. But this one is ok, too. Forget the stuff behind EOP, and only look at the differences between the grooves, based on straight lines.

As Jeffrey stated before, there's no real difference between moving a pin in an existing slot, or creating a slot by moving a milling tool along a part.

😉 Both tasks MUST be done by thickening a center surface.

[SBix26]

I didn't get good results with thickening surfaces, either, so I did it with sweeps.  The actual results will vary dending on the cutter diameter and the way in which the entry opening is cleaned out, but I assumed a cutter diameter the width of the slot, which is the most useful given that a pin nearly that diameter will actually be used in the slot.

Sam B
Inventor 2012 Certified Professional

Inventor Professional 2014 SP1 U3
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M

[dho · Accepted solution]

have any thought on dimensioning?

thanks.

http://forums.autodesk.com/t5/Inventor-General/can-INV-dimension-the-slot-which-was-generated-emboss...