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This task shows you how to display the number and name of the
components belonging to the active component as well as the properties of
these components. It also shows you how to save this data. |
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You can display the bill of material of the active component only.
Open the
AnalyzingAssembly01.CATProduct document. |
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Select Analyze > Bill of Material.
The Bill of Material dialog box is displayed. It is composed of
two tabs:
- Bill of Material,
- Listing Report.
The Bill of Material tab shows the different parts and
sub-assemblies of AnalyzingAssembly01 which is the active component.
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The Bill of Material does not show the possible representations
associated to the components.
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There are three main sections:
- Bill of Material: lists all parts and sub-products
one after the other,
- Recapitulation: displays the total number of parts
used in the product AnalyzingAssembly01.CATProduct,
- Define formats.
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Click Save As... to save this data. The Save
Bill of Material As dialog box is displayed. Three document formats are
available: .txt as text format, .html
as html format and .xls
as Excel format.
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Select the appropriate directory and enter a name in the
File name field. Note that the file generated will
contain the date of generation. For instance, if you selected the .txt
format, the document looks like this:
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Now click the
Define formats
button to customize the display of your bill of material. A new dialog
box appears, indicating the default format, i.e. AP203 format.
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To create the format of your choice, click
on Add. Format.1 then appears in the Selected Format.
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The Remove button is used for removing already existing
formats. |
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You can display the directories used for your assembly by
clicking the Search order option. For more about the Search Order
capability, please refer to
CATIA- Infrastructure User's Guide.
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Now, choose the properties you wish to display in the
Bill of Material section of the Bill of Material dialog box. To do so,
for example, select Source from the list Hidden properties and click the
show properties icon
to move Source
into the Displayed properties section.
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Likewise, double-clicking a property moves this property
into the section opposite. |
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Repeat the operation by adding Description to the
Displayed properties section of the Properties for the Recapitulation
frame.
The buttons you can use are the following:
moves
the selected property to the right scroll list
moves
all properties to the right scroll list
moves
the selected property to the left scroll list
moves
all properties to the left scroll list
moves
the selected property within the scroll list.
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Click OK to validate the creation of the new
format. The Bill of material: Display formats dialog box is closed.
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You cannot save the formats you create. Customized
formats are specific to your CATIA session. If you want to add numbers
in the Bill of Materials, you need to:
- open the CATProduct,
- select the CATProduct after having launched the
Generate Numbering functionality,
- click OK to generate a standard Numbering,
- then, open the Analyze > Bill of material. Select the
Define formats button and the Bill of Material: Define formats
dialog box is displayed,
- in the section called Properties for the Recapitulation, add the
"Number" property to the displayed properties.
The recapitulation list resulting in the Bill of Material is in the
wrong order according to the number, because numbering is applied first on
parts in the current product and then on parts in its sub products. |
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The Bill of Material now looks like this: |
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The Default Representation Source property is the
source of the default shape document. This property allows to show
the path to the file that contains the default shape associated to
the product node.
The Type property allows you to discriminate products
according to the following condition: if they are Assemblies or nodes
with no son.
The Quantity property allows you to distinguish
products according to the number of Instances that are contained in
the Assembly.
In this case the Default Representation Source of an
instance of a CATPart is the CATPart document file path.
Some nodes may have a default representation, others none. It can
be void for nodes (assembly parts) without any attached
representation, as in the example below:
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Click the Listing
Report tab. It displays the tree of the product using indents, just
like in the application.
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Check the Display
search order option if you wish to display the directories where
the different documents making up the assembly are located.
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To display other information in your report, select the
properties of your choice in the Hidden properties scroll list
and use the buttons as previously described to move these properties to
the left.
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To see the result, click Refresh.
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Use Save As... to save the report in the
directory of your choice. Only .txt format is available.
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Click OK in the Bill of Material dialog box to
exit.
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To know how to use your bill of material in your
CATDrawing documents, please refer to Adding a Generative Bill of Material
in CATIA - Generative Drafting User's Guide. |
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