Formed tubing (lawnmower handle)

[scottm]

On push type yard implements they usually use tubing for the handles/pushers etc. How would you go about modeling the end of the tube where they push the one side in to conform to the other side (hard to explain) so that it will mate with another tube. Below is a picture - top is a tube - bottom is the formed tube. This is only done on the last couple inches.


I could do a solid sweep or pipe and than remove the material, but that wouldn't really be an accurate representation. What I want is to make the hollow pipe and then deform it.


View attachment 699

 

[robertib]

I would use the warp function (in wildfire 2.0) - you can deform a section of a part without affecting the rest of the part.


The only problem is when you come to assemble to the warped model.

 

[scottm]

I'm going to try a swept blend if I can figure out how to do it...

 

[robertib]

Here is a blended thin protrusion that I created which looks like the part you want.


I'll put the details of how I did it in a separate post.


2005-03-10_095636_tube.prt.zip

 

[robertib]

First you need to create the sweep trajectory - I did this by creating 2 points & creating a datum curve through them.


Next, I used the Insert -> Blend -> Thin Protrusion. The blend options I used were Parallel and Regular Sec, and I used a straight attribute.


You need to draw on the plane that goes normal to the sweep. You need to mak as many drawings as there are places where the geometry changes - in this case 4 drawings were needed.


Draw a circle for the start point, and got to Sketch -> Feature Tools -> Toggle Section to move onto the second sketch plane.


This marks the end of the straight tube, so draw another circle of the same size, and change to another section.


This is where you need to draw the squashed section - I did this by using 2 semi-circles with different centres, connected at the ends. Repeat the drawing on the next section and exit sketcher.


Choose which side you want the material on, and select the thickness.


Finally, you need to select the depth of each section - ie. the straight tube, the compression down to the squashed tube, and the squashed tube itself.

 

[scottm]

Robert,


Perfect - I tried but I was using the regular protrusion and I didn't catch the toggle section thing. That's how I figured it should done but I couldn't figure out how from the docs.


Your a lifesaver - thanks for the help.


Scott

 

[scottm]

So I've got my part in... I went back in to add a section that I missed and ended up with this. Is there a way to identify the vertex points that get matched? I've tried redrawing the sections with no luck. It looks like a cobra... The sketches look very similar to your example.


View attachment 710

 

[dr_gallup]

It looks like you have a mismatch in your start points between sections. Pro/E is going to connect the start points between sections and then go around the section loops connecting the points.

 

[scottm]

That's what it looks like, but how do I (re)define the start point?

 

[huliyar]

redefine the sketch, select the vertex you want to be as a start point, then go to the 'sketch' menu, select 'start point' under 'feature tools'. if you repeat the procedure by selecting the same vertex, the direction of the arrow will reverse. you need to select similar points on all the sectionsas start points with samedirections for creating a proper swept blend.

 

[scottm]

OK, I did that, and now I've got rid of the twisty thing, but the cobra hood is still there. It's like its fitting a spline between all the points (is it?). Do I need to define the perimeter? Its pretty damned close. Should I do one sweep for the round part and a seperate sweep for the part that gets formed?