CAD CAM / Australia

philhuynh

Following on from last week, we will now take a look on how to use those custom made balloon symbols that we designed.

Now go into the BOM file in which you wish to create and set the repeat regions for BOM Balloons. This is done by going to the Table tab in the drawing ribbon, selecting the BOM balloons from the balloons group and then going to BOM balloon menu manager, select Set region to custom. Once you have done that select anywhere within the repeat region as shown. Next from the GET SYMBOL menu, you will need to select name and then the balloon option. This will acquire the custom symbol which was named balloon. To show the BOM balloons in the drawing view, click create balloon and show by view. After that select the view from the graphics window. Click OK from the custom balloon height dialog box to accept the default height values for the symbol used. Once you have done all of this, you should be able to see that the BOM balloons are now displayed on screen.

Now to use a different user-defined BOM symbol, go to the BOM balloon menu manager and select Alt Symbol. Once this is done select the balloon whose symbol is to bre replaced and then click okay from the select box. from the get symbol menu click on the appropriate name of the custom BOM balloon symbol. Click okay once you have completed adjusting the balloon height.

NOTE: In order to replace a BOM Balloon with a different symbol, the repeat region parameters displayed by the new symbol must match the old symbol. That is, if the original only displays the index in the balloon, the new symbol cannot display the index and the quantity together; only the index.

Congratulations, you have successfully use your own custom BOM balloons in PTC Pro/E Wildfire 5.0

Tags: BOM | Billing | Materials | Billing of materials | .drw | CAD | 3D | 2D | software | wildfire 5.0 | Pro/Engineer | PTC | Pro/E | improvement | symbols | file | Wildfire | 5.0

philhuynh

When creating Billing of Materials Sheet, it is important to create a different BOM balloons are displayed for a repeated region on the sheet to save you confusion or to make it stand out. This post will look at how to create and use custom BOM symbols. You will to firstly retrieve the file with .drw you want to customize for the session. Next you will need to go the Annotate tab from the drawing ribbon and expand to the format group and select the symbol gallery.

From the SYM GALLERY menu manager Dialogue box, click define and type in balloon as the new symbol name and press enter. Next click insert and then note. from here you are able to change the justification to Center and then click make note. Select the appropriate location to make the note and then type in \index\ in the Enter NOTE input window.  Press enter twice to confirm the changes. Click Done/ return once you see the new note appear in the window. Sketch the symbol Geometry as required using the sketch tools.

Note to remember: If text notes are enter with a backslash before and after them, they will become variable text notes. This means that you can arrange for preset values to be defined as symbol attributes and selected when placing the symbols on drawings. However if you want to use the same preset text in the symbol, do not add in any backslashes.

If text notes are entered with a backslash before and after them, they become "variable text" notes. Variable text allows for preset values to be defined as symbol attributes and selected when placing the symbols on drawings. Preset values may be used for each of these notes. If the text in a note is to remain constant when placed, do not use any backslashes.

Now that you that have finished creating you new balloon symbol you will need to configure the symbol General Attributes. By clicking on the Attributes from the SYMBOL EDIT menu manager, this will open up a new dialog box with the name Symbol Definition attributes. Make sure that you define the free, left leader and right leader placement types. Next Select the variable -drawing units as the symbol instance height option is available.Now you will have to configure the symbol Variable Text. This is done by going to the Var Text tab in the dialogue box and type in rpt.index in the preset values for index box text box.

Now complete the symbol configuration by clicking Ok, done with symbol edit menu and done with SYM gallery menu.

The Var Text tab in the Symbol Definition Attributes dialog box is used to define the parameter that will be called out by the variable text note. When the symbol is placed, the system will replace the variable text with the corresponding information being called out by the parameter. Any of the system parameters for drawings or user-defined parameters can be used.

For example, if one would like to call out component names in a BOM Balloon, the variable text can be defined to something like "\comp_name\", and the preset value/variable parameter would then be "asm.mbr.name".

NOTE: Note parameters cannot be used for the value of variable text.

Hopefully that will get you on the way of creating customized Balloon Symbols, Next week we will take a look on how to use that in the billing of Materials.

Tags: 5.0 | Wildfire | file | symbols | improvement | Pro/E | PTC | Pro/Engineer | wildfire 5.0 | software | 2D | 3D | CAD | .drw | Billing of materials | Materials | Billing | BOM

caddit

Checking the latest Pro/ENGINEER Wildfire 5.0 software kit, it appears that the only component of what was once the Pro/LIBRARY standard part library for Pro/E was the Mold Base. There is an online part library available from the browser favorites at http://www.3dmodelspace.com/ptc but each part needs downloaded individually.

After some checking, we discover that active account holders at ptc.com with support access can download most of Pro/LIBRARY in eight parts at http://www.ptc.com/cgi/cs/apps/SftUpd/SftUpdProd.pl (filter for "Pro/ENGINEER" related downloads; scroll to the bottom of the page) and listed under "WILDFIRE LIBRARY DATABASES". Although published with the original release of Pro/E Wildfire there are forward compatible with all releases and operating systems.

Installing these local part libraries require that we set up:

Pro/LIBRARY needs to be manually downloaded and configured as follows:
1: Create SYSTEM VARIABLE PRO_LIBRARY_DIR pointing to very top of library "tree"
    i.e. PRO_LIBRARY_DIR=/usr/local/ptc/libraries
2: Add matching lines in master (/usr/local/ptc/.../text/config.pro):
    pro_library_dir /usr/local/ptc/library
    search_path_file /usr/local/ptc/objlib/bin/config.pro
    SHOW_ALL_MOLD_LAYOUT_BUTTONS   YES
3: Create a top-level menu (Top-Level "index.mnu" File):
LIBRARIES
#
#
/objlib
BASIC LIBRARY
#
/mfglib
...

About .mnu files: The .mnu files configure "navigation" for browsing the library from Pro/E assembly component-insert, 2D detailing symbol-insert, etc. Subdirectories listed in an .mnu file will be shown with the description from the .mnu file, unlisted directories (like installation directories) will stay hidden. Folders in the library without .mnu files will show all directories present in that folder without any further descriptions.

(config.pro can be updated by a utility in the bin subdirectory of each part library. A few are not part libraries but symbol libraries which may find a different location)

At last look the LIBRARY files still available are:

MED-6XX-CD-330_2002490_CONNECTOR.zip
MED-6XX-CD-330_2002490_ELECTRICAL-SYMBOL.zip
MED-6XX-CD-330_2002490_GRAPHICS.zip
MED-6XX-CD-330_2002490_MOLDBASE.zip
MED-6XX-CD-330_2002490_PIPE-FITTING.zip
MED-6XX-CD-330_2002490_PIPING-HEATING.zip
MED-6XX-CD-330_2002490_TOOLING.zip

When we download and install one, we are asked to chose a target directory (should be a new directory that doesn't currently exist, directly under the library "root" location if we will be installing more than one under PRO_LIBRARY_DIR) in a dialog box:

Click next and we can choose what sub-libraries to install:

The library should install without much drama. Depending on which library we are installing, it can be used within Pro/ENGINEER design in a variety of ways. More information about configuring Libraries in Pro/ENGINEER can be found in "Introduction to the Libraries" (U00590197).

Tags: proengineer | proe | symbols | blocks | library | pro library | part library | standard parts | administration | caddit