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2) Hidden features won’t hide!


New member
I am running into the problem that when I hide a feature (in either part mode or assembly mode), it does not disappear from the display, even when I regenerate. I am able to hide entire parts, but not individual features.

Looking at the ProE help, it seems like I should be able to hide features, although it says "The following types of items can be hidden on the fly: ... Features that contain axes, planes, and coordinate systems". Does this mean that features that do not contain a coordinate system cannot be hidden?

Thanks for your help,

David Garber


New member
Hm I'm able to hide any feature (except patterns etc.) either from asm or parts, I'm not sure why you cannot.
But there is better way to achieve what you need. Its good practice to use simplified representations (both asm and parts), then you got saved rep of parts that you don't need (or features) and in any time you can turn them on to when you need them.


Hide does not hide solid geometry. That would require Pro/E to recalculate the shape of the part.

The following types of items can be hidden on the fly:

Individual datum planes (as opposed to hiding or showing all datum planes at once)

Datum Axes

Features that contain axes, planes, and coordinate systems

Analysis features (points and coordinate systems)

Datum points (whole arrays)

Coordinate systems

Datum curves (whole curves, not individual curve segments)

Quilts (whole quilts, not individual surfaces)

Assembly components


New member
Ok, to follow this: you can save views of a part with different features not displayed (as Isair referred to), but can youload these individual part views in assembly mode?

I think this has an affect on how to implement my design intent. I have a tube that is the main part, with different things going inside, but then there is a curved wall that connects to the tube and a space enclosure on top. I made these as one part with the tube, but if I will not be able to hide them it may be better to make them separate parts.

Here is a related question: when you want 2 parts to line up exactly (like for male/female connections), how do you implement this?I have found that it is very easy to do this is part mode because you can select all of the edges of one extrusion (for example) to be references for a second extrusion. But if you build separate parts, do you carefully record the dimensionsand build a new part, then in the assembly set assembly relations linking them? Or another way?


New member
If you create the part in the Assembly (Insert > Component> Create), then you can use features from the first part as references. Although, depending on what your assembly will be used for, how it will change in the future, etc., modeling features with external references that may or may not stick around with the part could cause problems downstream. In that case you'll want to create references in the top level assembly and use those. Do a search in this forum for Top Down Assembly Design to find out.


New member
It is much better to put separate parts in separate files; it's the way ptc has intended it to work best.

The best way to handle your related question is with the Top-Down technique using a skeleton model. If you have access to ptc's knowledge database, search for "using skeleton models to achieve top-down assembly design".

If it's too late to make such a change for this project then I suggest you create an assembly datum axis or straight curve to align the two parts.

Hope this helps.