Always make contact, as early as possible, with the person(s)
who will be doing the checking of your drawing before you begin. Do not wait until you start the drawing. Check with these people before you even start
the task. Do not underestimate this
advice. There are often particular ways
individual teams and personalities will want your drawing to conform to. Try to make this work to your advantage by
conforming to their way and perhaps a little flattery wouldn’t hurt either.
While in Assembly mode (double-click on your assembly),
select the Analyze pull-down menu, Bill Of Materials, select “Define
formats” button, add to the “Displayed properties” field with the |< icon;
remove a property from the “Displayed properties” field with the |>
icon. For example, the following may be
in the left hand column: Quantity, Part Number, Nomenclature, Definition,
Revision, Number.
See Post Insertion BOM
Editing for other detail regarding renaming Displayed Properties
See Preparing the
models for the BOM to prepare the Parts/Assemblies for the BOM.
While in your BOM drawing sheet(s) place the BOM into the
sheet’s Background as described below.
The BOM will first be inserted while in “Working View” mode
(Edit pull-down menu should say Background at the bottom) then Cut from the
“Working Views” so that it can be Pasted onto the Background of the sheet. The assembly selection step will be a similar
process as that described in View Creation
Wizard (Open your drawing, open your
top assembly…).
Insert,
Generation, Bill of Materials, Window, Tile
Horizontally, select the assembly from the Tree (in the Assembly file), pick a spot on the drawing sheet where
you want the BOM (wait for an approx. 5 second delay).
Then select the BOM, Cut (Ctrl-X), Edit,
Background, Paste (Ctrl-V) onto the Background.
See Printing – Display
Print Area to print out a rough copy of the entire BOM.
Back to Post Insertion
BOM Editing
Double-click on
BOM that was placed on the Sheet to enter modification mode. Before spending time “tweaking” the BOM make
sure you’ve spent adequate time with Preparing the models for the BOM
and Defining BOM appearance. Run some reference copies (see Printing – Display Print Area) for
whoever will be checking your drawing before conducting these “post insertion
edits” so that the “Post Insertion BOM Editing” will indeed be on your final
iteration. This is important since these
“post edits” will be lost if you ever decide that another “Inserting BOM in Drawing” is necessary.
While in modification
mode:
-Double
click on any text to modify it
-Drag the
“squiggly” row/column indicators to move the columns/rows.
Back to Defining BOM
appearance
Recommended to open part
files in their own window before populating the below “Product” fields. But if you do decide to perform in your
assembly file make sure that you expand the component branch so you apply the
following to the parts/assemblies and not the components.
Once a part is assembled to an assembly it is a
component. Expand the component to see its indentured part or
assembly. Right-click on the part or assembly and select Properties. The Product fields (within the Product tab)
will populate the BOM. The recommended
fields to use are:
-Part
Number
-Definition
-Nomenclature
-Source
Additionally the “Visualize in the Bill Of Material” radio
button should be selected.
IMPORTANT: Read
and understand Save Management. After completing the input to the above
Product fields make sure that Save
Management is reporting that the files have been “Modified”. If Save Management only says that the file is
“opened” then you will have to perform something to coax the file as modified
(e.g. open the part in it’s own window, double-click on one of its sketches and
immediately exit the sketch, close the part and if Catia notices it was changed
it will ask you if you want to save it.
You can answer Yes or No (to this window) but I would suggest answering
No and track all of your “Property edits”/”save verification” with the Save
Management method as described above.
This way you can more easily track which Property edits will require
additional “coaxing” until Save Management shows “Modified”. When you are finally confident that all of
your parts (that had their Property “Product fields” edited) will save, save
your top assembly (the assembly that all of your parts feed into) and all of
your parts/assemblies should save with it.
Reopen Save Management afterward to verify that all parts have saved
(their State would have changed from Modified to Opened).
Back to Inserting BOM in
Drawing
Back to Post Insertion
BOM Editing
Adding Format (into existing drawing)
Adding
Format (copying from one drawing to the
other):
Copying a format – Method 1 (out of an existing
drawing)
Copying a format – Method 1 (out of an existing drawing)
Open our drawing (h drive link shown below) where we have
dedicated sheets for all of our standard formats, arrow over to see other sheets (tabs), take note to
Page Setup (e.g. w=120, h=34.5), Edit, Background, select all
by using the rectangle selection trap ,
Copy (Ctrl-C), (Or see Copying a format
– Method 2). See Pasting a format for pasting the “Cut”
geometry.
-Return to your working views by selecting: Edit,
Working Views.
Make sure you’re in “Background” mode (i.e. Edit, Background),
File, Page Setup, select “Insert Background View” button, select
Browse, browse to the drawing (e.g.
template drawing) where you’d like to import a Background from an existing
sheet, Open, navigate to the desired
sheet in the Sheet pull-down menu, select Insert, OK.
Only the Background from the “template drawing” will be imported.
-Press Undo (Ctrl-Z) if results were undesirable.
-Exit Background mode (Edit, Working
Views).
See Copying a format. Open the drawing that you want to paste into
(if already open use Window pull-down menu), Edit, Background (no views
should be highlighted red), Paste (Ctrl-V).
-Return to your working views by selecting: Edit,
Working Views.
Assuming the format was added to correctly (to the
Background) as defined in Adding Format, Edit, Background (no views
should be highlighted red), double click on each text to edit.
-Return to your working views by selecting: Edit,
Working Views.
While in a Drawing do the following for each Sheet:
File, Page Setup, enter appropriate values in the Width and Height
fields (e.g. select “J U.S.Standard” from Format field, and enter 120 in Width
field, 34.5 in Height field) as described in Standard drawing format sizes, Resize
the drawing.
See Move multiple
views.
Create interruptions
(extension line break)
Always activate the desired view before adding text. This assures that text will be added to the
anticipated view and the text will remain in the anticipated position during
moving of views. If the desired view is
not activated than the current active view will automatically (and
inconspicuously) expand its view border to include the new text.
Activating a view (view border becomes red) by one of the following methods:
-Double Click on the view border.
-Right-click on the view border (or on view name in the
Tree), select Activate view.
highlight the leader, right click on yellow ball (at the end of the highlighted leader), select
All Around.
(so dimension extension lines break so as not to run over a
dim. Arrow),
-right click on a dim., dimensionname object ,
Create Interruption(s), select on two locations on the extension line to
define the break.
make a dedicated sketch, right click on the drawing view that
will show the sketch geometry, Properties, check the “3D Wireframe”
bullet and the “3D Points” bullet, OK.
Insert,
Annotations, Symbol, Weld Symbol, click on the screen
to define the arrow location, click
twice on the screen to locate the symbol, select the appropriate symbols,
OK…
Double click on weld symbol…
Ctrl-P (or File, Print), change to the desired
printer (in the Printer Name: field), change the Print Area pull-down menu to
Display, select the “Fit to:” bullet (Position and Size section), select Page
Setup button, change Width to 11, change Height to 17 (for a 11”X17” vertical
printout), OK, select the Preview button, if the preview clips some of the BOM
continue with step 1 below if not continue with step 2:
- OK (to exit Preview), select the Center button, adjust the Scale field, hover the cursor over the gray rectangle (with the “X” thru it) and drag the region to a new center, select Preview button again and judge again, repeat or proceed to step 2.
- OK (to exit Preview), OK to send to printer.
Back to Inserting BOM in
Drawing
Back to Post Insertion
BOM Editing
Keep reduced size prints proportional to the actual drawing
format size. Use the Measure icon to
measure the length of the drawing border.
Ctrl-P (or File, Print), change to the desired
printer (in the Printer Name: field), change the Print Area pull-down menu to
“Whole Document”, select the “Fit in Page” bullet (Position and Size section),
select Page Setup button, change Width to 11, change Height to 36* (for a 11”X36” horizontal printout), OK, select the
Preview button (all of the drawing should be within the red dotted lines), OK,
OK.
*Example: for a 66” long J
size (H=34”) print at ½ size: print at W: 33 H: 17, fit to page
(W: 36, H=11 seems to work well for many plotters [for J
sizes up to 120” long] and is legible).
A: 8.5 x 11
B: 11 x 17
C: 17 x 22
D: 22 x 34
E: 34 x 44
J: 34 x 55min (176 Max)
Adding
Projection View (to existing view)
See Drawing Views icon
group for location of Projection View icon and other “Projections” group
icons.
Activate (double click on) the parent view (activated view
border should be red), select the Projection
View icon, move your cursor to the desired position
(close to the activated parent view), left-click to accept view location.
Review For view
maintenance purposes.
See Drawing Views icon
group for location of View Creation Wizard icon and other “Wizard” group
view creation icons.
Open your drawing,
open your top assembly, Window, Tile Horizontally, select the
View Creation Wizard icon (if grayed out you haven’t opened your
top assembly), select one of the
Configurations icons on the left (e.g. “Configuration 1 using the 3rd
angle projection method”), Next, select another icon on the left (if additional
views are desired), Finish, This
next step is important if you want to link directly from the drawing to the top
assembly only: select a
component from the Tree (preferably from the 1st instance [e.g.
componentname.1; for commonality
sake] if more than one instance exists) before selecting a planar surface,
right-click the component you just selected from the Tree and select “Reframe
on”, now select a planar surface
from the highlighted component in the graphics window, next do one of the following:
-click anywhere on the screen (except on
the “view orientation” arrows) to
accept the default orientation
-or click on one of the large
arrows to flip the view orthogonally
-or click on one of the two curved
arrows to rotate the view about an axis normal to the sheet
Back to Inserting BOM in
Drawing
Back to To save the view
(adding custom views)
Back to Adding Projection
View
Back to View Creation
Wizard
Back to FTA & Drawing
views
Note: You can use your top assy always as
the assembly to pick the planar face of the view. But the key is to first select the model
(part/assy) from the top assembly’s Tree, then pick the planar face from the
graphics window. This way when you go to
“File, Desk” it shows links from the drawing view directly to the top
Product. This is often the preferred
linkage. Often preferred to have the
drawing directly linked to the top product only (see Desk).
The following (along with Removing components from view) assures
that proper view Updates with the minimum amount of view maintenance.
-View creation should be from the smallest model (least
number of parts). Thus, for a view
showing a single part, the planar surface selected to define view plane should
be from a part file (.CATPart). For a
view showing an assembly, the planar surface selected should be from the
pertinent sub-assembly (so as to minimize manually clicking off the radio
buttons as described in “Removing
components from view” below).
- Unlocking a view (right-click, Properties, uncheck
the “Lock View” radio button (under View Tab)
-Select them (left-click) from the Tree, although they can be
selected by the view borders
-Multiple view selection in the Tree: select first view (at
top of list), hold the Shift key as you select the last view (bottom) in the
Sheet’s Tree list.
Back to Move multiple
views.
Right-click on dimension, Properties, “Dimension Line”
tab, uncheck the “Symbol 2” radio
button.
See Drawing Views icon group for location of
Broken View icon and other “Break view” group icons.
Activate (double click on) the parent view (activated view
border should be red), select the Broken View
icon, follow directions in lower left of
graphics window….
-Don’t forget you can use Undo (Ctrl-Z), repeatedly until the
view returns to it’s “pre-broken” state, if undesirable results.
-To delete the Break, right-click on the break (so it
highlights), Delete.
Activate (double click on)
the parent view (activated view border should be red), select the Breakout View icon, define a breakout loop by left-clicking
(multiple points) on the portion of the view to be broken (see lower left of
graphics window if further direction is needed), double click to end definition
of the breakout loop.
-To
remove breakout: right-click on the view, viewname object >, Remove
Breakout.
Right-click on view, viewname object > Overload
Properties, select the component (that is to be removed) in the view, Edit,
uncheck both of the following two radio buttons: “Use when projecting” &
“Shown”.
See Selecting views. After the views have been selected (geometry
will be highlighted in each view) initiate the move by depressing & holding the left mouse
button atop one of the view borders (away from any entities), drag the depressed left-click to the
new location on the sheet.
-Other view movement options are available by right-clicking
on a views border and selecting View Positioning. For example, select two views (with Ctrl
key), right-click on view border, View Positioning, Element Positioning, place
cursor over the variety of Align options, select the
Move views to other
sheets:
select the view from the Tree, Cut (Ctrl-X), select the sheet that the view will
be moved to and Paste (Ctrl-V).
Recommended to move the views to an anticipated “empty” location (if
convenient) so that once they are moved to the new sheet they won’t be atop
other views.
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