I hve prblms usng Pro to make dwgs

[cad fool]

Hi, can you help Me?

I am trying to learn Pro-E on the fly (while working) and although I have learned alot on my own and from my past Solid-works experiance, I am finding the going very tough.
How do I?
Delete a setion view from the setion list
delete sheets
copy views, to show one wiew as a section(for instansce)
add a rev block
add a note with a leader pointing to a particuler feature any help would be welcome and greatly appreciated.

John

 

[acook]

Hey John,
<br style="color: rgb(0, 0, 255);">>Delete a setion view from the setion list

Not really sure what a "section list" is. I assume you are meaning removing a previously created section view (section name) from the drawing. In this case, you must remove the created section view from the drawing. Since you deleted the section view, I am assuming that you want a different one with the same name you just deleted. You may delete this "old" section two different ways (not the best interface in ProE).

***NOTE: These procedures will NOT work in Wildfire 1.0 and I am unsure about Wildfire 3.0!***

1) If you have another cross-section in the drawing, double-click it to bring up the view properties. On the left-hand column, select "Sections", in the "section list" use the drop-down box to select the old section view (should contain a red "X" by the name) and right-click to select "Delete from model". Click "Apply" and then the "Ok" button to proceed.

2) If you have no other sections on the drawing, goto any of the remaining views and double click it to open its view properties. On the left-hand column, select "Sections". Temporary set the radio button to "2-D cross-section" and select the desired view from the "section list". Right-click the old section view name and select "Delete from model". Click the "Cancel" button to proceed.

This is shown below,

View attachment 2646
>delete sheets

Goto Edit->Remove->Sheets... and a prompt will appear in the dashboard requesting the sheet number that you want to delete. Enter the sheet number and press <ENTER> or sleect the "Green arrow" in the dashboard.

>copy views, to show one wiew as a section(for instansce)

Not really sure what you mean by this. I don't think I have ever copied a view before. It may be possible.
<br style="color: rgb(0, 0, 255);">>add a rev block

If by "rev block" you mean the space which contains a brief description of all the changes made in each revision level (as well as the date and the person who made the changes), there is really no way that I know of in ProE to "add" one. In all the companies I have seen, they all just create one manually. I believe this is differenent than SolidEdge and SolidWorks which provide revison block templates. ProE (to my knowledge) does not.

Here is an example of how we handel the revision block (I am not saying this is the "best" way, personally I don't like it). The notes and the lines dividing each revision level were all manually gnenerated.

View attachment 2647
>add a note with a leader pointing to a particuler feature...

The expaination on how to do this is long, but once you do it once you will pick it up pretty easily.

Goto Insert->Note...

A menu manager will appear such as the one shown below.

View attachment 2648

Ensure that for selection "1" that "With Leader" is chosen. Selection "2" is how the leader line will interact with the slected entity (e.g. if "Normal Leader" is selected, the leader line will ALWAYS be normal to the entity). Chose "Make Note" for selection "3" to continue.

Another menu manager will appear along with a "Select" dialog for choosing the entity to which the leader will attach. These are shown below.

View attachment 2649


View attachment 2650


Ensure that selection "1" is "On Entity". You may choose the symbol "style" which will appear on the selected draft entity in selection "2" ("Arrow Head" is standard). For selection "3", first select the deisred entity on the drawing (the selected point on the entity is where the leader will first appear, but you maychange this latter) and then click the "OK" button as shown on the dialog above. Finally, select "Done" for selection "4" to continue.

ProE will now ask you to select the location of the note (the actual text) on the drawing. Select this location and type in the desired note in the dashboard. Once you finish entering in the note, a final menu manager will appear, select "Done/Return" on it to finish.

Hope this helps.




Edited by: acook