extrusion of a closed shape along a curve

[Hans11]

Hi all,

What I want to do: I try to extrude a circle along a curve (as a path for the circle) to get a bended tube. But I always get an error message.

My way: In the 2D scetch mode, I create a circle. Then as a new shape I create a line.Afterwards I chose "sweep protrusion", choose first the by left mouse click the curve (path), activate it with the green tick. Second I choose the the circle and suddenly get an error message that the ordner could not be executed.

So to start with: Is it correct, to create both, the circle and the curve in the same plane?

Any further idea, what might be wrong?

best regards

Hans

[nominus38]

Firstly, you should begin having just the curve you want to follow. Then, draw your circle as a sketch on PLANE NORMAL TO CURVE. Then connect the center of the circle to the end pierce point on that curve. This should do it for you. FIrst step select the curve, next select the circle.

But you should consider using FRAME to do this, it'll be a bunch easier.

[Hans11]

Thank You for reassuring me, that I need to use two perpendicular planes.

Unfortunately I do not know what "FRAME" is, as I use a german version and do not know what the german counterpart is.

But now I had some success, as I was able to extrude the circle along a singular line. But I want to create a frame of a tube along a rectangular. So I used the 2D command to create a rectangular as the path in the new plane. And I got the same error message again. When I remove 3 of the 4 lines creating the rectangular, I get the extrusion as expected. But even if I leave 2 of the 4 lines creating there rectangular, I get the error message.

What principle did I harm?

[Hans11]

Some additional information:

When I put the close shape (the crossection of the tube) into the XY-plane. And I put the rectangular (path of the protrusion) into the YZ-plane, then I get this error message. It works if I only use that line of the rectangular (along the Z-axis), that is perpendicular to the frame. But the error occurs for the line that is in the plane of the tube's cross-section. Quite obvious ....

But how can I make the tube's cross-section follow a curved line, which necessarily has a component in one of the cross-sections plane?

[Hans11]

Explaining all that, helps me to find a bit closer to the solution, i assume.

I found, that the problem is that I put the tube's crossection to the corner of the rectangular path.

If I remove the final line of the rectangular path coming back to the center of the tube's diameter (thus being in the plane of the tube's cross-section) and leave the other 3 lines, starting perpendicular to the tube's cross-section, the tube follows these 3 path-lines.

I just cannot make this part close at the end.

How to do this?

thanks for Your patience.

regards Hans

[hawcad · Accepted solution]

Hi @Hans11

first of all the FRame Environement will be found in ASM and in the GErman version it is called "Strukturrahmen" or "Rahmen"

Here You only need to define the path curve (line in Your case) and take a already defined frame profile to drive along

And if You do not want to use the frames then let me sa, that Your method was done in the wrong order.

First You have to define or select the drive pat curve (line) and afterwards the cross section according to the Smart Ribbon Bar and the request from the info bar (follow them step by step)

Another hint would be to go into the help for this feature I'm confident that there will be ceratin viewos available to look at.

One possible reason for the failure of that feature might be, that You have to consider that any corner can be build.

If the cross section is to close to the corner how should that profile be moved along the drive curve?

Hope this helps

[nominus38]

@Hans11in order for you to sweep a protrusion, the path must be all tangent with itself. So you can't go thru a rectangle or any angle unless you add a radius at the intersection.

[hawcad]

HI @nominus38

so IMHO this is not true.

The path curve can also be sharp edged.

There is no need for a tangent continue situation

See picture above

2 sketches

First with 3 lines edged and second is the profile with a rectangle

[Hans11]

I believe, I found the cause and the solution:

The 2D-curve created with the rectangle is a closed curve. I.e. if I put the cross-section, which I want to protrude at the corner of the rectangle, with line no.1 perpendicular to the cross-section,the full path continues into the second, third and forth line segment. This final segment comes back to the origin of the path. This makes my start-point ambiguous to solid edge (while it is never ambiguous to a human mind). This way this path is not acceptable to Solid Edge.

What needs to be done is using the line tool and not the rectangle or circle tool and create an open path with a clear start and end point. To finally close the tubing, as I want it, I need to create an open path, as close to my required path, provoke the guided protrusion. Afterwards I need to close the gap in a second step by protruding the end crossection by linear protrusion into the startsegment of the tubing.

I put this answer to not leave the question open.

If somebody knows a more elegant way, more answers are desirable.

best regards Hans

[Hans11]

Dear Wolfgang

You suggested to use the assembly environment (instead of the part-environment) and there the Frame, called in Rahmen in german. Generally it sounds promising, but unfortunately I didn#t find this Frame ...

Where should I look?

best regards

Hans