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Rotated slots through a tube

Dave H

Senior Member
Been away from Alibre for a while and I'm rusty (and older!)
I've been trying to figure out how to model two rotated slots 180 degrees apart through a piece of tubing. The ends of the slots have to be rounded as if the
slots were cut with an end mill. (cuz they will be) They have to line up so a dowel would go through both sides of the tube and be able to follow the slots axially when the
tube is rotated. Similar to a hollow barrel cam. Anybody willing to help with this?
I am using Expert 2018 version if that matters. TIA!

Dave
 

HaroldL

Alibre Super User
I was working on something similar a few days ago. The best way I could figure out was to create a Helical part with full radius ends then use Boolean Subtract to create the slot in the tube. It is important to create a circular pattern of the Helical part BEFORE accepting the Boolean Subtract.

You may need to make several adjustments to the Helical part to get the slot as required in the tube.

As an example, here is the part I was experimenting on. Hope it helps, well, maybe not, I see you are still on 2018.:(
:( Well since you won't be able to open the model I made a short How To video to describe how I made it.

 

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  • Slotted Tube.AD_PKG
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Dave H

Senior Member
I was working on something similar a few days ago. The best way I could figure out was to create a Helical part with full radius ends then use Boolean Subtract to create the slot in the tube. It is important to create a circular pattern of the Helical part BEFORE accepting the Boolean Subtract.

You may need to make several adjustments to the Helical part to get the slot as required in the tube.

As an example, here is the part I was experimenting on. Hope it helps, well, maybe not, I see you are still on 2018.:(
:( Well since you won't be able to open the model I made a short How To video to describe how I made it.

Thank you Harold. Your video example is exactly what I want to do. Everything you did on the video I can do in 2018. In fact, that was maybe going to be my next attempt. I was just hoping there was a better way rather than going the boolean route. I got it mostly done using the helical cut, but couldn't figure out how to get radiused ends. I was thinking along the lines of a 3D guide curve and maybe a lofted cut.
Anyway, thank you very much for the help. I get the feeling that is the way I will end up going.
 

HaroldL

Alibre Super User
@Dave H, Glad to help out. It took me a while to get my head out of SolidWorks to finally figure this out in Alibre. Like I mentioned in video, the fillets could be added after the Boolean but as long as I had the part open I just added fillets to it and saved a step in the tube model.

@Ken226, thanks for the comment. I thought it would be easier to show and describe the steps I took rather than starting from scratch. That would have been a much longer video.
I suspect the new 3D Wrap will get a lot of use for some of your models.
 

Ken226

Senior Member
I can't leave a challenge like this without having a go at it, via a different method.Untitled.jpg

A contour flange in sheetmetal. Unbent, slots extruded throught, then rebent.

I started running into trouble when i set the sheetmetal thickness over 1/8" though. I kept getting a bend radius error.
 

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  • New Sheet Metal Part (1).AD_SMP
    503.5 KB · Views: 3
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Dave H

Senior Member
I can't leave a challenge like this without having a go at it, via a different method.View attachment 35898

A contour flange in sheetmetal. Unbent, slots extruded throught, then rebent.

I started running into trouble when i set the sheetmetal thickness over 1/8" though. I kept getting a bend radius error.
This idea went through my mind also, but having done very little with the sheet metal metal I really didn't know where to start or how to place the slots in the flat pattern so they come out right when rolled.
 

HaroldL

Alibre Super User
Yup, that 'll work too. It seems that using sheet metal has been the go-to for several operations.
But for those that don't have Expert it's out of the question. I do hope that the new 3D wrap will be available in all versions of AD and Atom.

I checked out your SM part, I reduced the Min Bend to .01 and that seems to have fixed it. I was able to get the thickness up to .250". I also simplified the sketch for the Contour flange, just another sketch method that you may employ.
 

Attachments

  • New Sheet Metal Part (1).AD_SMP
    448 KB · Views: 5
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Ken226

Senior Member
This idea went through my mind also, but having done very little with the sheet metal metal I really didn't know where to start or how to place the slots in the flat pattern so they come out right when rolled.

I took the radius to the OD of the tube x pi, as the distance halfway around the circumference.

After unbending, I sketched a reference line along the unbent part = in length to the radius x pi, midpoint centered at the center of the part. The created a slot centered (rotated 25°), on one end point, then pasted a copy of that slot at the other end point.
 

Ken226

Senior Member
Yup, that 'll work too. It seems that using sheet metal has been the go-to for several operations.
But for those that don't have Expert it's out of the question. I do hope that the new 3D wrap will be available in all versions of AD and Atom.

I checked out your SM part, I reduced the Min Bend to .01 and that seems to have fixed it. I was able to get the thickness up to .250". I also simplified the sketch for the Contour flange, just another sketch method that you may employ.

Thanks Harold.

The "Minimum Bend" setting is what I was missing. Excellent info to know

Thanks.


It renders up into a fine looking widget...

untitled.3.jpg
 
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Dave H

Senior Member
With the help of you both I was able to get this done! Rust and all.
I did it the way Harold first showed due to my lack of sheet metal skills. Only thing I was not able to do as Harold did is to circular copy the helical cut. That did not show up in my Design Explorer. So I had to insert two helical bosses and constrain them a little differently. But it worked fine. Thanks to you both!

Now to consider renewing maintenance......??????? I don't make any money with Alibre anymore,since I retired, but maybe one last time?

Slotted Tube.png
 

HaroldL

Alibre Super User
Looks good. The circular pattern is actually created inside the Boolean Subtract before you accept the Boolean. Watch the video again and check out the DE, you can see that the circular pattern is a child of the Design Boolean. Creating patterns of Boolean features is something that puzzled me until I figured out that you can create patterns before accepting the Boolean.
 

Dave H

Senior Member
Looks good. The circular pattern is actually created inside the Boolean Subtract before you accept the Boolean. Watch the video again and check out the DE, you can see that the circular pattern is a child of the Design Boolean. Creating patterns of Boolean features is something that puzzled me until I figured out that you can create patterns before accepting the Boolean.
Ahh, must have missed that little detail.
 

HaroldL

Alibre Super User
I suspect jobs like this are going to be alot easier when V25 comes out! It won't be long now.
You are absolutely correct. And working with some of the Wrap options comes up with different results that need to be fully documented for any meaningful Help documentation.
 

Ken226

Senior Member
You are absolutely correct. And working with some of the Wrap options comes up with different results that need to be fully documented for any meaningful Help documentation.
"Project" seems to work great.

But i can't get wrap to work with anything but really simple geometry. The same sketches that work fine with "project", fail with "Wrap".

Text Wrap Fail.jpgWrap Logo Fail.jpgAlibre Logo Projection.jpg

Projecting seems very good, but either Wrap needs some work, or as you mentioned, they need to educate us on it's limitations and requirements.
 
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DavidJ

Alibre Super User
Staff member
I seem to recall that element of sketch being close to edge of face can be an issue.

Suggest that you report via feedback buttons on the Home Window of the beta - just to make sure Development is aware.
 

HaroldL

Alibre Super User
I seem to recall that element of sketch being close to edge of face can be an issue.
I reported that Wrap failed for me when the sketch was closer than .138" to the part edge. Your example appears much closer than that.
I sent a video along with my report so the issue was well illustrated for Development.
 

Ken226

Senior Member
On my test file above, the text and the A logo were separate sketches. Both failed wrap, but for different reasons.

The A sketch failed, according to the error message shown in the pic above, because it's "difficult geometry".

The text sketch shows an "engulfs geometry" error, so that one may be too close to the edge.

I reported the issues via the little red frowny face cartoon button.
 
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