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How to hide planes

dveljkovic
6-Contributor

How to hide planes

Hi all,

I do not know how to hide these datum planes aka not to show at all. I do not want to use layers because they propagate all the way through to the part level. I discovered, by pure accident, that when CTRL-ALT keys are pressed, Creo hides them all.So, does anyone know to how to hide these planes by default?

HIDE.png


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11 REPLIES 11
Constantin
13-Aquamarine
(To:dveljkovic)

If these datums were created on part level they should be hidden using layers on part level. If they are assembly datums you can hide them via layers on the assembly level, there is no propagation...
Maybe you need to specify your problem a little.

dveljkovic
6-Contributor
(To:Constantin)

Constantin, when plane is set to be a datum plane, it shows itself on screen even when button "plane visible" is off. I need to know if there is a setting somewhere in Creo that I can set so it does not show on screen unless I choose "plane visibe=ON". And I do not want to use layers to solve this issue.

Constantin
13-Aquamarine
(To:dveljkovic)

Hi Danilo,
I think it will only be possible using a layer.
Layers are not evil, they are friends

dveljkovic
6-Contributor
(To:Constantin)

I agree with you about layers, but I do not want to use layers for a simple plane visible on/off issue.

Inoram
13-Aquamarine
(To:dveljkovic)

I am confused about what you are asking.

If you just want default planes not visible when you start Creo you can set

display_planes no

in the config.pro, but this is only setting the default position of the switch on the graphics toolbar.

dveljkovic
6-Contributor
(To:Inoram)

Matt, does this setting "display_planes no' hides also datum planes? The answer is NO.

Using Layers is presently the only answer. It can be less painful to include layer rules in the models to automatically move add the set datums to a layer and remove them from other layers to make visibility control easier.

dveljkovic
6-Contributor
(To:dschenken)

David, I would have no problems with layes if they do not propagate all the way to every detail. So when I open the detail, datum planes are also gone and that is very bad on some commercial items where I cannot constrain them without using planes.

Layers can be hidden or shown on a per-component basis. Visibility of the set datum planes (aka 'shown' in the rules collector) can be independent of other datum planes. Any combination of layer display is available at any time.

PTC layers is badly named when compared with the way layers work in other applications. PTC should call them named lists. In most applications each item has a layer number associatated to it - each item can be on only one layer at a time.

In PTC software an item can be on multiple lists, and need not be on any list; lists can have rules that gather items on the list based on membership of other lists; selections can be made using lists. Using layer lists to control visibility of items is a minor capability, but one that has been reliable for the situation I think you are describing.

...and you wonder why people don't like "layers" in Creo

There are some other underlying rules behind showing and hiding things that overwrite layers. Such as trying to hide the primary solid object in the part file. Unfortunately, these tagged datum planes are one of them. At least, they seem to be when tagged with the ISO style datum tag.

It gets even worse when you use the newer ISO style datums (also recommended by ASME). They have a behavior all their own. We had discussed this at length.

The 1st thing I recommend is not making the default datums tagged datums (for lack of better way to define them). If you assign the datum to a surface, they behave a little better. Or create datum planes specifically to use them as GTOL datums and nothing else. Don't ask me why, but it does make a difference.

Then I found out that these new style datums have a mind of their own which is somehow related to their use in drawings. A datum I couldn't hide for the life of me in the model suddenly would disappear when called to show in a drawing. Now try bringing it back! That is why you don't want to use the primary datums.

The old style tags are a little more forgiving. I even had trouble deleting the new datum tags at one point. I had to change them to the old version and then they could be deleted.

You are certainly not alone in this. A search of the forum on "datum tag" will get you more information.

I think the term "persistent" somehow applies to these. I think I remember they not always following layers either, at least not the new style.

And from the past, yes, even in the old Pro|E times, tagged datums were a true issue in large assemblies where they were persistent as well.

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