exploded views

[17566]

Solid Edge v18, I have set up assembly with a lot of hardware, I am greating a exploded view to show up on a draft file. I would like most of the hardware to disappear. I TRIED in the assy to hide hardware, but still shows up in the draft file. I also tried to use bind command this did not work. Is there a easy way to do this????

 

[beachcomber]

Hi 17566,
Solid Edge displays all parts of the model in the drawing view regardless of whether the file is saved with the display of some parts turned off, unless you specifically tell it otherwise.
There are 3 ways of doing this.
First way is to reate a Display Configuration in the model, then use this configuration when the drawing view is placed (or you can set an existing drawing view to use this configuration).
In your exploded view hide the parts you do not want to see, then Tools>Display Configurations and save the view with a suitable name. Then when you place the view select the Configuration name in the drop-down box. Note that you will still get the option of which orientation you want the view (top, iso etc.)
Second way is to use the draft view properties.
RMB on the draft view and select Properties.
On the 'Display' tab you will see the assembly structure tree under Parts List. If you click on any part in the tree you will see a tick box to the right labelled 'Show'.
Uncheck the box to hide a part (or sub-assembly) and then 'OK'. Update the view to see the changes.
Third way is really a combination of the first two.
Create a View Configuration as above, the on the draft view properties set the Cofiguration of the existing view to match. You should see the new config listed in the drop-down at the bottom of the 'Display' tab.

bc

 

[PatCouture]

Beachcomber said it all!

I just want to add that if you are making an exploded view then the best way would be to simply hide the hardware while you are making your exploded view, then when you get out of the exploded view environments SE will automatically save those settings as "explode (username)"

Patrick

 

[17566]

I am using solid edge V18. I am working in part file. I have sketchs in the part file, that I need, is there a way to bring it over to a draft file????

 

[PatCouture]

Absolutely

Once you have a drawing view of the part, go into the properties of the view and in the upper left corner there is a button under the tabs that is called "part list options" that will enable you to show the sketches, then you must be able to select it and click show on the right as if it was a part by itself.

I hope I'm being clear enough

Patrick