Sweep Analysis?

[Soloboss]

I created a new part. It's a swept protrusion having the trajectory created from two lines and two arcs on a single plane. Now I'd like to know the actual length of the trajectory from end to end. I don't find an analysis tool that recognizes the lines and arcs. We don't have the piping or cable add-ons or I'd use those, but I'd expect the system to know what it just created. I expect that I'm simply asking the question incorrectly, but I don't see the option I want under the Analysis button.
If what I'm asking is impossible, what's the key to creating a line/arc/spline trajectory that I can analyze?
Sorry for the newbie questions, but I'm getting no useful answers here at work.
Soloboss

 

[loughnane]

It sounds like you just want to measure the length of a curve (your trajectory).

If that's the case, you are in the right place. There is a "length" option under analysis. (In WF2 it's in a drop down box, in later versions it's right in the main analysis menu).

If I'm mistaken and you are actually looking for something else, please include an image.

Chris Loughnane - Product Design

http://www.pdnotebook.com

http://www.twitter.com/DesignNotebook

 

[Soloboss]

What you stated is correct. I want to know the full length of the sketch (trajectory). Using the Analysis LENGTH command and passing the cursor over the sketch sections, the sections don't highlight. The curves and straight sections are not selectable. I tried the same analysis using the swept surface but the surface isn't recognized either. I could calculate the arcs using the radius dim, but I can't find the swept angle or cord length or any information other than radius size. What am I missing?
If I did this correctly, there should be a shot of my screen showing my "mission impossible".

 

[loughnane]

Gotcha.

First problem is that you can't use the measure feature inside a sketch. So you have two options.

You can create the sketch first as a separate feature, and then once the sketch feature is closed you will be able to select the curve with the measurement tool.

The measurement tool might only grab a section of your "path" if it is made of multiple entities (line, arc, spline, etc.). If that is the case, select the first entity, hold shift, and select the rest. once they are all selected, press CTRL+C, then CTRL+V to make a "composite curve".

The other option, if you want to get the dimension in sketcher, is to use what Pro calls a perimeter dimension.

this place explains it pretty well.

http://www.proengineertips.com/sketcher/tips-dimensioning-techniques-in-pro-e-sketch-4.html

let me know if this solves your problem.

Chris Loughnane - Product Design

http://www.pdnotebook.com

http://www.twitter.com/DesignNotebook

 

[mjcole]

Step by step instructions cause Pro/E is still stuck in the past.

I find that it helps adding a column for Feature Parameters to Model Tree and enter VALUE as the Parameter to show.
After defining the Curve Length measurement you can hit the AddFeature button and save an analysis feature. You'll have to edit this after the fact if you want to use Value as the parameter name.

Easy method - Use Analysis > Measure
Option1 Curve/Chain
* Hover over sketch curve and Right Click until entire loop is selected

Option2 Chain
* Hold down CTRL Key and pick 2 neighboring entities in sketch
* Hit Next in side menu and then select after entire loop highlights

Option3 Feature
* Pick sketch feature from screen or Model Tree

Which ever above option you used hit the Add Feature button. Enter a name for the Analysis feature A1 or CurveLength.
After analysis feature is Created you can Edit Definition
and select from options to create Parameters or change parameter names. I usually use VALUE as the parameter to create because you can show multiple values for different Analysis types.

The Default Parameter name is Length or Area or Distance depending on Analysis. To change this expand
[+]Result Params tree branch and the Parameter Type
[+]LENGTH
Double Click Parameter Name and enter the value for the Name and hit Enter then hit the check mark to Finnish the Feature definition.

Difficult Method write Relations in sketch relating to reference dimensions for line lengths and arc lengths

A1len = pi*rsdA1(sdA1/180) where
rsdA1 is Radius Sketch Dim value for Arc 1
sdA1 is angle of arc.

For a Slot like yours
d## = L1 + L2 + A1 + A2

If you write a relation for dimensione length sd## of a construction line you can edit the Dimension while in the model and add Text in properties as

CURVE LENGTH
@D
so it's visible in sketch and model

I prefer the former method with the feature because it's easier to accomplish and will update if the Sketch Feature changes.

Michael