Show the internal sketch

[ptc-5177357]

Hi,

I am started working in Creo elements 5.0.

I have created a feature with an internal sketch and I want to use this internal sketch to give geometric constraints for the next sketch, but I could not make visible or select the internal sketch. Please anyone tell me that how to make visible or use this sketch to give geometric constrain for the next / other sketch.

Thanks in-advance.

Regards

Perumal

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[Patriot_1776]

Create a stand-alone sketch prior to all the features you want to drive with the sketch. I do this quite often to get the relationships I want.

[dgschaefer]

Internal sketches do not create geometry that can be used outside that feature. Although you can 'internalize' an external sketch, unfortunately there is not way to 'externalize' an internal sketch even in Creo 2.

You'll need to do as Frank suggested - create a new standalone sketch ahead of the feature, redefine that feature to use the new external sketch and then use that sketch to build your other geometry.

[Patriot_1776]

You can kind of cheat and save the sketch in the existing feature, and use that to create the datum curve prior to the feature, then redefine the feature to use that geometry, but yeah, no easy way. That's one of the major things I DON'T like about SW, is all the external sketches with limited usability that you're stuck with. In Pro/E, I use internal sketches (and datums) almost all the time, unless I need them for multiple features. Like I said, an internal skeleton.

[TomD.inPDX]

Although Frank and Doug pointed out a serious oversight on the part of developers, you can do two things to capture data from internal sketches:

1: You can add datum points to internal sketches to use outside the sketch. When datum points within internal sections are visible (visibility enabled), you can reference them with other features such as subsequent sections.

2: You can build relations with any internal section's dimensions be they driving or driven (reference) dimensions. Not as straight forward as I like, but you can make the relation feature driven instead of part driven but it takes a few mouse-clicks to get there. This is why it is often under-utilized where simple relations are not created although they really should be in order to make changes easier in the future. It is pretty much a sustainability requirement. If PTC could make it easier to do on the fly within the next level section, it would probably get used more.

Be aware, however... you cannot always add the datum points later in time. I don't know why this is, but I have often found I needed this at a later part of the design and I was locked out of the capability.

Personally, I like clean modeling trees but internal sketches and even internal datums create limitations. You really need to choose carefully which are right for the given situation. Often times, you are well served by creating a "master sketch" or some kind of control sketch that manages "envelope" requirements. This can be changed on the fly with new requirements. A pseudo skeleton model if you will.

[dgschaefer]

External sketches do clutter up the model tree, but they also make redefining features more difficult in that from the feature dashboard you cannot get into the sketch if the sketch is external. Adding access to the external sketch from the feature dashboard would be a welcome enhacnement.

[Patriot_1776]

Excellent point. Sometimes I've added CS to a sketch, like for a connector, to identify pin 1 and easily constrain at at assembly. Having that ability is nice, though the "axis point" feature had already been around a while, though it was unavailable in sketcher. So, that's nice having the points.

I'm using an internal skeleton now, in fact, to relagte a face to a pin hole to a slot, all created in different solid features. this way I can easily control the cam slot profile to the pivot pin hole, to the actuating face.

[gkrishna]

I have attached a screenshot of what was shared on different public forum,about generally how your model tree should be (grouped).not hard and fast rule but essentially good.

[TomD.inPDX]

That list is a great guideline.