taper in square part

[larry53]

I had a problem at work drawing a square part that had a taper. I was trying to show a 10 degree taper from the square part. It was to end up .100 diameter at the end. The square is .375. Everytime I was making a taper square and not a rounded taper. I need someone to explain how to make a taper on a square part. I am using Inventor software. Thanks Larry

[Rube]

Hi Larry...so you want a .375" square on one end and a .100" round on the other (like the attached picture)?
To do that you need to use the Loft feature. This requires two sketches. Draw your .375" square then finish the sketch. Then create a parallel offset plane to draw the circle on(if you want a 10degree taper you would need to do a little math to determine how far to offset that plane from the original (.78"). Or if you dont really care about the taper angle, but know the length of the part, offset the plane that far from the original. Draw the circle then finish that sketch. Call the "loft" tool and select each sketch as a section, and it will do a smooth surface transition from the square to the circle. You will need to select if you want the output to be a solid or a surface (I assume solid in your case).

It took me longer to type this than to actually do it.

[larry53]

No what I meant was square turned round at a taper ending in a .100 dia. In other words picture turn a piece of square stock in a lathe at a taper. It would be round from the square to the end of the part. This is what Iam having trouble drawing. Thanks for your effort and time spent.

[Rube]

huh, ok...sounds like all you want is a cone? If the part can be made in a lathe, "revolve" is the command you want. Sorry if I am totally misunderstanding what you are looking for.

[mcphill]

huh, ok...sounds like all you want is a cone? If the part can be made in a lathe, "revolve" is the command you want. Sorry if I am totally misunderstanding what you are looking for.

Actually I think he wants to subtract outside of a cone from a square stock. I don't have Inventor, but am sure this can be done. Probably wouldn't help to post a SolidWorks screenshot, though it would confirm the shape you are trying to make.

[MarkWink]

Is this the shaped required (see attached pic)?

There is alot ways to draw this, this one was drawn with two sketches and two extrudes.

[larry53]

The shape is correct except the taper continues through the square stock.

[mcphill]

Like this, right?

[larry53]

That is what I was meaning.

[Rube]

OH, now I get it..duh sorry. still simple, two extrusions. Make your .375" square bar first the total length you need. then draw your .100" circle on the top. when you then extrude the circle select "intersection" (this leaves only stuff that is within the square and the cone). for the extents of the extrude you can either play with the distance untill it goes far enough to get what you want, or just select the opposite end of the bar as the "to" plane. click the "more" tab and define the 10 degree taper angle.

Hope this helps.

[larry53]

Thanks very much for the help. I try it and had no problem.
Thanks again. Larry