Slot on Radius

[cnelson]

Good Day All,

I have a cylindrical part that is a radius along its axis. Hard to explain in words so I have attached the part file.

Anyway, I am trying to apply a slot for a label along the Z axis of part. The slot needs to be of relatively equal depth for its entire length.

I've included a PDF showing the approximate location and orientation the slot needs to be.

There must be a simpler way than multiple work planes, points, and axis being applied...or is there? Thanks for any assistance.

CCN

Slot orientation

[mcgyvr · Accepted solution]

Your pdf didn't get included so its difficult to see what you really want..

Also what version of Inventor do you have..

I "think" that using the new extrude "distance from face" option is what you want..

My sketch in blue is on the origin plane in the center of the part.. Then using the "distance from face" option in the extrude dialog I was able to create a slot on the face of the part to whatever depth I wanted..

Like this..

[karthur1]

You mean like this?  I just sketched a slot and then extruded using the new "distance from face" option.  May not be what you are wanting.

[mcgyvr]

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@karthur1 wrote:

You mean like this?  I just sketched a slot and then extruded using the new "from surface" option.  May not be what you are wanting.

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@karthur1   Beat ya!!!

I only posted an image because I see they are still on 2017 and I don't remember if that was added then or in 2018...

[cnelson]

Hi and thanks for replies.

The PDF was actually just the attached photo with red line sketch.

I am using Inventor 2017. Does this new feature exist in that version?

Thanks.

[I_Forge_KC]

If the tube shape is cylindrical or conic, why not emboss this?

[andrewdroth]

Ah Looks like Emboss is not supported on a barrel like shape. Bummer.

[andrewdroth]

Since Extrude from face isn't an option in 2017, this is how I would do it.

[cnelson]

Thanks for trying...I did try that too.

[karthur1]

Emboss works just fine on a tapered surface here.  I am using 2018, but it should work the same in 2017 as well.

Kirk

[I_Forge_KC]

Yeah, I only have '16 here so I wasn't sure on the surface specifics (it looked conic to me), hence my qualifier there.

Emboss enables this kind of functionality going back many releases.

[cnelson]

It does but the depth is not equal. The sketch would still need to be created on a work plane closely angled to the tangent where the slot is being created. Does that make sense?

Thanks.

CCN

[I_Forge_KC]

Wrap to face is your friend.

[JDMather]

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@cnelson wrote:

It does but the depth is not equal. 

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Extrude-Cut to an Offset surface would be uniform depth

or

Split and Thicken-Cut are other techniques that will work depending on Design Intent.

I would post example of the Extrude-Cut to Offset surface, but I noticed that your sketches were missing dimensions and when I added dimensions - they did not make logical sense.

These two techniques could be used back 10 yrs or more.

(Do not require 2018.)  (Do not require cylindrical or conical faces.)

[karthur1]

Can you show us a cross-section of what you want the slot to look like? A hand sketch is fine.

Is this a machined part?  If so, how do you plan on machining the slot?

[cnelson]

Thank you all. I will try some of your suggestions. I am in the process of downloading 2018 to try some of the new features available.

[cnelson]

I will when my 2018 download is complete.

It is a machined part and I will leave the slot machining technique to the experts. I am certain they will have some questions.

Thank you.

CCN

[karthur1]

If you are cutting it with an endmill, the bottom of the slot will be flat and 90° to the sides (unless you are using a tapered endmill).  It will not be on a radius, which is what you will get if you try to model it using the "distance from face" option.  If that is close enough for you, then go for it.... but, technically, that is not correct.

If the endmill is 90° from the center axis, it will look like the attached model.  The slot will be slightly different if the end mill is on the same angle as the taper.  There will be a small flat at the end where the endmill "plunges" into the part.

Hope that all makes sense.

Kirk

[cnelson]

Yes, that makes perfect sense. Still in midst of 20GB download.

Will give it a try when complete.

Thanks.

CCN

[johnsonshiue · Accepted solution]

Hi! This is an interesting case. It is a bit open-ended meaning there are multiple ways to interpret the design and create the geometry. Attached is an example using 2017. I mainly use surfaces to create the desirable cutout. Please let me know if more information is needed.

Many thanks!