Permanently hiding sweep sketches

[cwilkes]

Got an issue,

I sketch my sweep trajectory in a new sketch. I then start a sweep feature and select the sketch as my trajectory, sketch the section, etc. and end up with the sweep I want. After this process, my sketch still shows in very obvious blue on my gray part. I can open the part and hide the sketch, but upon reopen, it comes right back. HOW DO I KEEP THIS HIDDEN? So simple but it's driving me crazy. I know about making the trajectory sketch embedded in the sweep, but i'd rather have it be a separate sketch..... just not visible.

Thanks

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[LukaszMazur · Accepted solution]

After hiding sketch feature (or any datum/surface feature, to be precise), go into View tab and click Save Status in the Visibility group to save layers status display and then save a part. This way you'll have sketch hidden next time you open the part. You can also switch Model Tree to Layer Tree, right click in Layer Tree to bring up context menu and select Save Status from the menu (and also save the part after that). Both commands work the same way and save layer display status for part.

And if you're not using Creo Parametric but Pro/E, the setting is in View > Visibility menu.

[cwilkes]

perfect, thanks for the quick answer.

[LukaszMazur]

No problem, glad I could help

[AndréLuizM.Guim]

Chris Wilkes, you need to hide (Layer Tree) more before you must hide your superfice scan that you want to hide and save the module tree hidden layer.

1 - View

2 - Save Status

okay

or

1 - Show

2 - tree Layer

3 - Right Button

4 - save Status

[Patriot_1776]

The best way is to use an internal sketch for your sweep (or other) features, that way it is automatically hidden and is not cluttering up your model tree.

You could also create a layer for layout sketches and hide the layer.

Were you a solidworks user, perhaps?

[LukaszMazur]

The best way is to use an internal sketch for your sweep (or other) features, that way it is automatically hidden and is not cluttering up your model tree.

This is not possible in Creo Parametric - PTC has removed "old-style" Sweep feature (from Insert > Sweep > Protrusion/Surface/etc.) and merged it with Variable Section Sweep, therefore it's required to sketch trajectory as a separate feature (or use existing geometry). For older releases it's indeed right and I think it's better to use internal sketches whenever possible, but sometimes it's just not an option.

[TomD.inPDX]

Yes, this seems to be inconsistent. With helical sweeps, you can still define the trajectory in the feature, but not sweeps. Lame

[Patriot_1776]

Wow, that sux. One of the many reasons I've chosen to stay on WF4....... In fact, I was forced to do some dwgs in creo today......hating it.

[pimm]

I'm seeing that the construction geometry comes back if you set your Save Status in one part and then later Merge this part into another.

Save Status is greyed out in the new part which the original model which this was Merged into.

Is it possible to hide all these curves in a model that includes a Merge?

[TomD.inPDX]

Save status is only active -if- there is a change to be saved. You could try creating a layer for the sketches and adding them, then hiding this layer. Now you should be able to save that status.

[pimm]

I was able to hide the unwanted curves and sketches in general part models by making a change to the model as you suggested. I ended up with only stamping curves shown.

The reason I went through the trouble was because I need to export stamping detail in my top and bottom IGES'd mold dies.

This brings me to another issue however. In bringing the part model into the mold model as a reference it appears to take over all curves which negates the exercise of getting this hidden in the part model in the 1st place.

I was upset specifically about this until I exported the die IGES with curves (as I still needed the stamping). It did not export any curves at all. This makes it good in the fact that all the construction geometry wasn't IGES'd, but bad in that I could not export the stamping curves built in the model that was imported into the mold model.

By any chance is there a way to import into the Mold model a what you see is what you get representation and once that is done export out of the mold model a what you see is what you get?

[TomD.inPDX]

Wouldn't that be nice

As I often avoid this, I'm going to suggest maybe using the family table options. I don't have the mold option but have merged bodies and it does take on several of the model properties. Why it would take on curves is beyond me. I know you can hide things in display states, but I doubt that will do anything in the mold's merge function. It could be worth a try.

Have you looked at the IGES export options? There are many you can set in config.pro (INTF stuff) but you can also go into the options editor when you create the IGES file. I think you hit F4 to have it show you all the viable options. You should be able to export the curves in IGES.

[pimm]

Thank you Antonius, I'll have to check out the export options you suggest in IGES. I'm already getting some of the trial by fire.

Creo often adds layers of complexity that are difficult to dodge. I wish you could merge the simplicity of use with the ZW software (that we also use) with the tools and control you can achieve with Creo.