Where is the "Start Point" definition for sketcher trajectories?

What type of feature are you making when encountering this, a Swept blend? To shift the start point in a swept blend section this should work ( I have not used Creo 9 yet so it may have changed).

With a sketch active

1. Select the desired vertex for the new location of the start point
2. Right Click > Start Point

• ​Repeat steps to flip the direction of the Start Point
• If sketched sections exist before creating the blend feature, the user can move the start point outside of sketcher mode (with the blend dashboard still open)

If you want to flip the direction on a sweep trajectory, use the RMB to get the flip option.

To set an interior point on the sweep trajectory for the sketch plane, use the options tab.

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@ByDesign wrote:

I'm looking for what used to be called "Start Point" in sketcher -- or some other way to tell Creo where to put the sketch on a trajectory.  I see the  Setup > Feature Tools > Start Point, but it's always grayed out, not available.  I want Creo to put the sweep sketch at the other end of the sketched trajectory.

 

In a search, I found another post about this, but the answer is for a much older version, so doesn't seem to work with Creo 9.  Is it another silly hidden magic click?  Or a completely different process?  Thanks.

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Hi,

In Creo 9.0.2.0 I place mouse cursor on magenta arrow and click left mouse button. This action moves magenta arrow to opposite endpoint.

Notes:

• my first feature is Sketch containing single spline
• my second feature is Sweep using Sketch

Thank you @tbraxton .  What you say is kind of what I was originally expecting.  I tried so many combinations of clicking and LMB, MMB, RMB.  In the sketch, or outside the sketch, Click and it changes color so you think something is happening, but the colors are apparently meaningless.  I see in the images below (your second post) -- which are very interesting, thank you, but I can't duplicate that behavior with the RMB.  There may be changes for Creo 9.

I appreciate the time in sending the sample images.  I messed with the options as you show, which is interesting.  I can see how that might be useful sometime.  The options do provide a way to move the section, but it does not change the direction of the trajectory -- which IDK, maybe it's meaningless in light of the answer noted by @MartinHanak .  You can see what Creo thinks is the direction by looking at the 70% point in the attached image.  Creo thinks the start of that curve is on the right.  In previous versions, you could define the start in sketcher by choosing an end and defining it as the "Start Point".

The solution by @MartinHanak does solve the issue of which end to place the sketch.  Thank you.  The curve direction does not change, so the 70% point does not change, and I can't figure out how to define the "Start" or Zero end of the curve.  That's what I was originally looking for, but maybe moot based on the Magenta arrows.  It still leaves the question of defining the curve start.  If anyone knows how that is now defined, I'm really interested to know.

As a side note, I'm just flabbergasted yet again at the horrible UI.  How would that magenta arrow click be found?  I read the document linked in the top right of the feature ribbon for more info, and did not find it.  Actually the documentation is very poorly written if you really want to find something.  It's command based with limitations, and almost nothing on application.  After the answer from Martin, I searched the document again.  No mentions of Magenta, Arrow, Color, Red, Pink, ... PTC, if you're listening, when you have a HORRIBLE UI with so many hidden little gems, you have to be really thorough in documentation.  Better to have good UI, but since you've failed at that, PLEASE make the documentation and search worth using.  Make the context sensitive help (little flyouts) worth reading.  Adding hyperlinks in the tab boxes explaining -- for instance what the "Options" are and how they apply (Not just lists of commands like in the current docs).  Add links to the training (within Creo or at least from the documentation) so customers can learn.  I searched for a solution for a while and found almost nothing.  Google was more helpful than PTC's docs - which is sad.

Thank you @MartinHanak for knowing, and sharing, this lovely tid-bit.