Explanation of Terminology - Tangent Continuous

[Wiemannironworks]

I am increasingly exasperated by the term "tangent continous" used to describe an error in a swept protrustion and the inability to locate the definition anywhere within SE V19's help section. What do I need to correct on my sketches to eliminate this error? All of my sketches are connected as far as I can make them. I have a simple 90 degree turn located in one sketch plane and SE refuses to sweep the profile around this turn.

Any help would be appreciated.

 

[fredericmenage]

What happens if you try a sweep with that path but with a very small (centered on path) circle as the cross section ?

If it works, it means that your cross section is too big and self-intersects at some point along the sweep.

If it still doesn't work, make sure you have a tangency (symbol=circle) at each endpoints in your path sketch. Especially if you are using multiple paths or sections.

Also, if your path is built using more than one sketch. Combine your path into one entity use the derived curve command and make sure you select that feature as your path.

HTH,

Fred

 

[Wiemannironworks]

I don't think I can use the Derived Curve Command for my paths as I need the Sweep to follow my path exactly.

I have a simple path in one plane that makes a 90 degree turn. I have a second sketch that makes a compound angle from the first sketch. I have connected the sketches using the Blue Dot command and SE tells me that the distance between the two sketches is 0.0000 inches. I can sweep the single planar path from either end using a plane normal to the curve, but SE won't make the compound corner and keeps telling me the first path is not tangent continuous (whatever that means). A derived curve radically alters the path sketches into a different shape that is not what I need.

 

[swertel]

To perform that sweep, you need to have a fillet between the two sketches that form the compound angle and the radius of the fillet is dependant on the profile being swept.

--Scott

http://wertel.eng.pro

 

[Wiemannironworks]

Can I use a fillet with a radius of 0. I need the corner to be sharp. If so, how do I go about filleting two separate sketches?

 

[donyoung]

Hi

as Ferd already did point out *all* segments your path is
constructed of must be not only connected but must show
the tangency symbol. In other words make each line tangent
to the next. A 90 degree (sharp) corner will not work
with a protrusion (self intersecting) unless you profile
is indefinitly small ;-).

dy

 

[donyoung]

Hi,

the name should have been Fred, I apologize for that typo

The only thing to get a sharp corner is IMHO to cheat a bit.
For I don't know wahr profile you try to sweep I've put
a small sample here

Sweep

You have to unsuppress the features

BTW: when you get "... coincident faces .." as error for any sweep
then a curve on the path is too sharp for the profile to sweep around

HTH

dy

 

[Wiemannironworks]

When you say that a 90 degree corner won't work for a swept protrusion, you mean it won't work if the path is in two different sketches? It works if there is a 90 degree turn in a single sketch but I can't get it to make the turn between the two sketches. I am building a section of mitered pipes that form a compound angle. This is mostly an exercise just so that I can get everyone on board with the design as it was pretty difficult for me to spatially organize it in my head. I also need to generate an accurate drawing of the piece that contains the multiple miters so that I can break it down into machinable setups.

 

[donyoung]

Hi,

I just discovered a small misalignment so the corner was
not accurat. The file has been replaced, so the above link
is still valid

dy

 

[Wiemannironworks]

I cnanot get you Sweep to run. It opens with errors in the two Protrusions and the Cutout and cannot identify why it won't generate the Protrusion.

 

[donyoung]

Hi,

did you unsuppress both protrusions and the cutout?

dy

 

[Wiemannironworks]

I see it now. When I saw the "universal" crossed circle icon I thought it meant that the protrusion had failed.

Thanks to all of you guys for your help. I think I have a work around on the project that avoids the compound miter afterall.

 

[donyoung]

Hi,

when a feature fails it either shows a red exclamation mark
or a grey arrow. The crossed circle just tells that this
feature is currently 'out of service' ;-)

[...]
I am building a section of mitered pipes that form a compound angle.
[...]

Isn't it possible to use the 'Frame' feature for for this?

dy

 

[Wiemannironworks]

I am unfamiliar with the Frame feature.

 

[onefjef]

I don't know what sections you are trying to sweep but I didn't have any trouble sweeping round and quadralateral shapes even with sharp or 90 degree corners out of plane. Use the derived curve command.

Jef