Is there a way to display sketcher lines outside of sketcher mode?

[mperkins]

Hi All,

I'm using Creo 3 and am unable to find a solution. I am wondering if it is possible to display sketcher lines while outside of sketcher mode when creating a part. Let's say you have a simple cube made from an extrude and you then select a face of that cube to draw on--a line for this example's sake. Once I click okay and exit sketcher mode, the line is not visible unless I hover my cursor directly over it. In my line of work this can sometimes be a major annoyance and I'd like to see sketches outside of sketcher if possible. Is there a way to change this?

Thanks

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[TomD.inPDX]

You might also try removing all appearance changes from the render tab.

It is an option in one of the appearance manager windows.

If your system behaves differently from what I outlined above as a simple test, you could create a support case.

[mperkins · Accepted solution]

I just found the solution to my problem. While looking into the various configuration settings and files that Creo uses, I found my Creo admin's config.sup file that we use. There was a setting in there called "shade_with." The description for this setting is:

shade_with

curves*, no

Displays datum curves on shaded objects.

I changed it from "no" to "curves" and it immediately resolved the issue. I believe that I didn't resolve the issue previously because I was making changes to config.pro and if I'm not mistaken config.sup has has priority and will override any conflicting settings to the config.pro file. I also do not think any settings from config.sup are displayed in the Creo configuration editor, so it wouldn't have come up when I was trying to find keywords. In any case, it is doing what I expect now.

Thanks for the help everyone.

[Tmetcalf]

Thank you for sharing your final solution Maxwell.

Best,

Toby

[dschenken]

The configuration editor has a pull down that lists the places it gets info along with 'current session'. This way you can see all the options that are brought in by each file that is loaded as well as see the overall effect (except for .sup each loaded file overwrites the previous in-session settings) It also allows editing the exact file you want; by default that is current_session.pro. Changes to the .sup generally require restarting Creo if they are to over-ride current .sup controlled options.

That has got to be the most misleading config option and a poor decision to put it into the .sup.

It inspires a config rant. on how poorly done the config system is, which I will take elsewhere.

[psobejko]

Well, you learn something everyday.  This one has some prank potential.

[TomD.inPDX]

Interesting find, Paul.

I do not know where the config.sup file comes in but I always keep an "original" desktop link to know I am booting "Ceo out of the box".

This helps eliminate any config issues.

Thanks for posting!

[dschenken]

The .sup file is supposed to allow company admins to ensure a consistent product by placing them in the not-overrideable config.sup and placing it in the Creo startup path. How it often ends up is the admin gets a complaint from one user and, rather than investigating it, they find an option that ruins the Creo experience for everyone to hide the original problem.

My favorite is an admin thinking to force some standard mapkeys into .sup. Since .sup locks in -only one- value for the config option, not only does it define exactly one mapkey, it makes certain that no one else can create them. (Unless PTC has changed this in Creo specifically; that was the way it worked for a very long time.)