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As you know, you can set two different work modes prior to performing
tasks in this workbench:
- The Design Mode uses the original component
documents.
In other words, geometry is selectable and workbench commands are
available if this mode is activated.
- The Visualization Mode uses documents in cgr format.
Only the external appearance of the component is visualized and the
geometry is not selectable, which may be useful when you deal with
sophisticated assemblies with large amounts of data but only need a few
components to work on. Using a cache system considerably reduces the time
required to load your data.
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This task illustrates the use of the Visualization Mode and more
precisely one way of improving the performances of the product. |
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- Make sure that the Work with the cache system option is
selected (by default, the cache is not activated).
See
Cache Management for CATProduct and CATProcess Document.
- Make sure that the Automatic switch to Design mode option
is selected.
See
General settings.
- Make sure that the Compute exact update status at open
option is manual.
See
General settings.
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Open the
AssemblyConstraint07.CATProduct document.
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When opening assembly documents in
Visualization Mode, the Status Unknown icon
is always active, because the application cannot identify whether the
assembly is up-to-date or not.
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Looking closer at the specification tree, you
can notice that the nodes are expandable, components are displayed with
the following format: Instance_Name [Document_Name]
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Click the + symbol of each component nodes.
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Looking closer at the specification tree, you
can notice that the nodes are not expandable, components are displayed with
the following format: Product_Name (Instance_Name). |
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The assembly has performed the update status:
the Update icon
is grayed, the assembly is up to date.
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Information contained in the CATPart document
about annotation, publication or contextual part for example, can be
loaded, but not the affected geometry. An information is then displayed
on the object icon in the specification tree indicating that the geometry
is not loaded or eventually broken (i.e. an exclamation mark mask on each
published element, a question mark mask on each annotation, etc).
Note that for this sample nothing has been loaded.
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Click the Offset Constraint
icon
to define an offset constraint between Part.5 and
Blue_Part.
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According to the selected options:
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As you are moving your cursor onto any
geometrical element of the parts in Visualization Mode, you can notice
that an eye symbol is located next to your arrow.
This indicates that the geometrical element can be constrained, but take
into account once it is selected.
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Select a geometrical element or a published
geometrical element loads almost the entire CATPart document in session,
furthermore for publication of Generative Shape Design
objects like point, line or plane, you have to complete yourself the
entire loading of the CATPart document before select the published
element (i.e. by clicking the + symbol on the part node).
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When setting the constraint on the Part.5,
the CATPart document is loaded and appears under the related component. |
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Then on the Blue_Part, the CATPart
document is loaded and appears under the related component. |
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Once the constraint is set, take a look at the
tree. |
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The fact that the application resolves
constraints while working in Visualization Mode is possible only if your
document contains data created from Release 10, and not using previous
releases.
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The application resolves constraints set from
published elements from Release 11.
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Contextual parts in Visualization Mode remain
in this mode if they are up-to-date, on contextual publication all
version, on contextual geometry from Release 11.
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When CATPart are modified and saved outside of
the CATProduct context,
or when CATPart are partially loaded, modified, saved and unloaded in the
CATProduct context,
the constraints cannot be updated in Visualization Mode
anymore.
You need to load CATPart in Design Mode in the CATProduct
context and force the CATProduct save.
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Setting the Design or Visualization Mode
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When you open a product document in
Visualization Mode, you can define a mode specific to a component
using the following contextual commands: Representations >
Visualization Mode or Representations > Design Mode. |