Sketching inside a cylinder

[dutchfisher2005]

Hello,

I'm designing a two stroke cylinder. I'm trying to sketch the exhaust port and duct. I'm finding it difficult to sketch the outline of the port onto the cylinder wall and then extrude cut the duct. I have tried a 3D sketch on a plane at both the angle of the duct (20 degress from Horiz) and front plane. However then i try the extrude cut the edges of the port turn up at the surface of the cylinder wall. I want the top of the port flat as in the sketch.

Not sure if i'm going about this the right way.

Using SW 2008 Sp5

Thanks

 

[Mitsu50]

can u post a screen shot?

 

[Updraft]

Use a 2D sketch on a plane and Extrude-Cut to make the ports.

- - -Updraft

 

[dutchfisher2005]

Done

 

[dutchfisher2005]

Updraft, tried that, but the curve of the cylinder wall made the top line curve up at the edges. I also tried a wrap (which solved the curve up) but i could not extrude the wrap. Dont think you can extrude wraps in SW

 

[Eltron]

I assume we are looking at the sketch normal to the profile? It almost appears that you are extruding the cut at some angle other than orthogonal to the cylinder. Could that be the case? What options are you using when you make the extruded cut?

Dan

http://www.eltronresearch.com

Dan's Blog

 

[dutchfisher2005]

.. to add

if it where possible, i would sketch on the horiz, extrude cut to surface (cylinder wall surface) then extrude that cut (from the cylinder wall) again at 20 degrees down downwards for the duct.

Not possible it seems.

 

[dutchfisher2005]

Eltron,

Yes normal to the sketch, the centre of the sketch is exactly on the cylinder wall axis (28 radius from the bore (and part) centre.
The extrude cut is bi-direction. The cut away from the cyilnder (downwards forming duct) is fine, the reverse dir is the problem.

I've only been using SW for 3 weeks, this is the first time i've been really stumbed

 

[Eltron]

What happens if you extrude a solid body (don't merge it) and do a combine/subtract? Does it look the same?

Dan

http://www.eltronresearch.com

Dan's Blog

 

[dutchfisher2005]

While responses are gathered, here's another question.

The exhaust duct changes section shape as it proceeds. I think I know how to do this using a lofted cut with a profile. However the 2 duct merge into a single duct.

Do i have to add a sketch at the end of the lofted cut to continue the extrude cut with a single duct?

 

[dutchfisher2005]

Eltron

Nope thats the same.


I did try to draw a 3D sketch over the the weekend directly on the cylinder wall using the shadow of the wrap as a template.
I gave up as it was just too difficult and I dont think that would extrude cut anyhow.

 

[Eltron]

I think you'll have to post the part for us to dig any deeper.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[dutchfisher2005]

Thanks Eltron

 

[Eltron]

I see. If I'm understanding correctly you want the second direction of you extruded cut to be normal to the sketch which is normal to the cylinder wall. Correct? Just share the sketch between two extruded cuts instead of trying to do it in one operation. Check the attached image to see if this is what you need.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[dutchfisher2005]

Correct.
I don't know how to 'share' a sketch.
Looking at the image, it appears as I want it viewing at that angle. I see you've added a 'cut extrude' to the tree, need to examine how you did that. Possiblily best if you post your modified part

Thanks

 

[Eltron]

I'm on 2011. Just click on the sketch that you used for that first cut and do another cut in the other direction. SW will automatically share the sketch between the two features.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[dutchfisher2005]

OK I got you, but no, that puts an angle in the duct. Not what I'm after. The duct must be straight from the cylinder wall all the way to the outer casing. The only other way I can think of is to draw the sketch with a curve that equals the cylinder wall curve as produced by the current sketch, so being a straight line on the extrude cut. That's not a very good solution as the current sketch is just a test and the final edit of the part would require rejudging the curve every time I adjust the sketch.

Is it possible to 'convert' a wrap or the intersection of an extruded to surface outline to a 3D sketch and then extrude from there?

 

[dutchfisher2005]

... ahh, I've just dug out an actual production casting. Looking up the exhaust duct towards the cylinder it has a compound curve at the apex of the roof of the duct and the port in the cylinder wall to produce a straight top to the exhaust port. Oh dear!

How in world am I going to reproduce that?

 

[CorBlimeyLimey]

Not sure how your last post affects what you are after now, but per the previous posts;

Use Sketch80 to create a Wrap on the bore
Use the Deboss option set to 100mm
Use the Pull Direction and select the line drawn in 3DSketch23

 

[dutchfisher2005]

CorBlimeyLimey

Excellent! That's perfectly how I wanted it. Thanks

Now all I have to do is continue the cut with a varying section shape and merge the 2 ducts into a single. I'll have a play with what I have now and come back if I get stuck.

One other note. Having used Autocad paper model in the past to obtain the area of these ports, I can't find the same tool in SW. I need to see the area in the sketch, and the area as produced by the wrap. The volume of the duct would also be handy.


Thanks again, I learned alot today.