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ptc-54934771-Visitor
1-Visitor
June 25, 2014
Question

swept blend

  • June 25, 2014
  • 6 replies
  • 10161 views

I have created an elbow as a swept blend. It starts out as a circle and ends up as a circle.

I'm apparently doing something wrong.

Again.

Please see the attached file.

The issue is that after the circles are blended, they are no longer circles but splines. I can't measure it in model space and can't dimension it in drawing space.

What am I doing wrong here?

Thanks.


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6 replies

D
dschenken1-Visitor
1-Visitor
June 25, 2014

Probably nothing. Sometimes geometry is promoted to a higher level of abstraction.

You might create sketched datum curves and create use-edge references in making the blend or add a sketched datum curve at each end that is anchored to the edge to give you something to dimension to.

You should still be able to show the arc dimension for the sketches on the drawing, but I can see where you might not be able to see the arcs that are in the sketch.

P
ptc-54934771-VisitorAuthor
1-Visitor
June 25, 2014

for fun, I created another swept feature consisting of two identical circles on opposite ends of a straight line.

This should give me a cylinder, right?

Same result - the measure tool won't measure it and in a drawing, I can't create a dimension.

In my earlier example, there are four sections, all circles. The first two are the same and the last two are the same. So I should have an elbow with cylinders on either end.

I don't understand what you mean by arcs. The only circular element that isn't a complete circle is the trajectory and I can see that just fine. And it's the only one I can put a dimension on.

T
TomD.inPDX17-Peridot
17-Peridot
June 25, 2014

Works for me...

blend_drawing.PNG

P
ptc-51247661-Visitor
1-Visitor
June 26, 2014

In your example I would do the cylinders at both ends of your tube using revolve or extrude and then blend only the section between them, selecting the resulting edges instead of sketching.

This I believe will also allow you to control the result better, as for example you will be able to add or remove tangency at either end.

P
ptc-54934771-VisitorAuthor
1-Visitor
June 26, 2014

another work around for something that should work out of the box.

Looks like this silly software turns the arcs to splines. How clever is that?

P
ptc-54934771-VisitorAuthor
1-Visitor
June 26, 2014

Yes, I can add those dimensions too. But mine don't come in as diameters and you've dimensioned to hidden lines!

Bad draftsman! Bad! <spritzes water>

Patriot_1776
Patriot_177622-Sapphire II
22-Sapphire II
June 26, 2014

You're not going to be able to measure (distance I assume?) on the blend because Pro/E doesn't know WHERE on that changing surface to measure, because you didn't tell it. In modeling mode you can query-select points on the surface. If you want dwg dims, put in a datum plane and use the interestion of that and the part to give you hard points to measure to.

An SPR is not needed, different/better technique is.

For this, honestly, I'd use a VSS, and in the curves defining the shape you can put geometry points wherever you want to measure to, AND the VSS will give you better control anyways and assure tangencies where you want 'em.

P
ptc-54934771-VisitorAuthor
1-Visitor
June 26, 2014

Not distance, but diameter. It should know, after all, I told it!

How should I modify my technique?

Really, this is simple and shouldn't be so hard - starts out as a circle, ends up as a circle. How come I can't measure it? (I know, it's a spline, but why the devil is it now a spline?)

I strongly disagree - a SPR IS needed. This is seriously broke and needs fixed.

I want to look into the elbow, from both ends, and put a diameter dimension on the diameters. Shouldn't need to add planes. There is already a plane there - my sketch is drawn on one - the section is normal to the plane/sketch/trajectory.

It works for Antonius. I'm presuming that he used my model. Why doesn't it work on my system? Antonius, what date code are you using? Is this a bug in my version? I don't have the authority to update my system, so for the time being, that's out.

What is this VSS you speak of? Creo help doesn't recognize it.

P
ptc-54934771-VisitorAuthor
1-Visitor
June 26, 2014

Ah, Variable Section Sweep. (Should have done the homework. Will have to look into that. I'm sure the help file will explain it.)

Really?

for a simple elbow?

Will I be able to measure the beginning and ending diameters?

Patriot_1776
Patriot_177622-Sapphire II
22-Sapphire II
June 26, 2014

A comparison for fun. The VSS is a little easier, I think, less sections to sketch, and you have more control over the geometry as well. What you can't do with a VSS is reverse curvature or switch between a straight line and curvature or vice versa.

FS_TEST_ELBOW-01.jpg

P
ptc-54934771-VisitorAuthor
1-Visitor
June 26, 2014

Thanks Frank. I'll have a look at these.

T
TomD.inPDX17-Peridot
17-Peridot
June 26, 2014

In general, people that have used Pro|E for a long time and use driving dimensions throughout drawings have learned long ago that we create sketches and dimensions solely for using them in the drawing. Sketches may even be created to have a driven dimension available in the drawing but created in the model. What is more difficult is to consistently have the arc of the spine echoed in the drawing as a centerline so the radius dimension has something to point to.

As for the surfaces or edges of the blended feature not having primitive information available, that is something we long understood as a limitation. Somehow I defined it, so somehow I can access the data I entered.

There are some occasions that policy forbids use of driving dimension on drawings and that only driven drawing dimensions are allowed. Considering Pro|E was never intended to be used this way, means that the policy is not in line with the software (that never happens!). I have the luxury of making drawings however I see fit. And I find myself using both methods and still remain perfectly associative on the overall shape and size of the object I document. But I do often find myself changing the model to suit the need in the drawing. This could well be improved.

T
TomD.inPDX17-Peridot
17-Peridot
June 29, 2014

Just for the sake of completeness... and something new to learn...

If you have access (probably requires maintenance):

http://learningexchange.ptc.com/tutorial/3336/utilizing-solid-bend-and-flatten-quilt-functionality-in-creo-parametric

flatten_quilt_deformation.PNG

B
BrianMartin13-Aquamarine
13-Aquamarine
June 29, 2014

Just FYI, nothing on the Learning Exchange requires maintenance (unless something has changed in the last 6 months). Learning Exchange is a totally free service.

Thanks,

Brian

T
TomD.inPDX17-Peridot
17-Peridot
June 29, 2014

Thanks for that clarification, Brian. It always wants me to log in and it doesn't remember my logon info. I wasn't sure what it is bouncing the credentials against.

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