Update VAA-Variants

Drawing > Save/Reference > EditCL > Update part variants

Variants in VAA_Format which are managed in HELiOS, will obtain a version number when they are changed. If you load a drawing that contains a VAA variant, HiCAD will check whether this variant has been changed recently. If this is the case, a corresponding message will be displayed:

If you want to update the variant in the drawing, activate the checkbox for the part and click OK.

To update part variants subsequently, select Drawing > Save/Reference > Part... > Update part variants .

 

Important:

The check is only possible for variants that are managed in HELiOS and had been inserted in the drawing with one of the following functions:

	Insert part, via DB document master (2-D/3-D)
	Insert part, via DB article master

 

Version numbers are assigned as follows:

• If the geometry of a variant managed in HELiOS is changed, and the geometry change is saved with one of the following functions:
• Save to variant, via document master data or
• Save to variant, via part master data ,

the version number of the variant will be incremented.

• If a variant managed with HELiOS is changed via the Variant Editor, only the version number of the changed sub-types will be incremented.

 

Please note:

• The update behaviour of variants can be preset in the Configuration Editor, at System settings > Referencing > HELiOS > Update variants. The default setting is Ask user.
• When you open a drawing containing variants, the check for changed variants can only be performed if the corresponding variants have not been opened in the Variant Editor at the same time.
• Parts which were inserted as variants from HELiOS into the drawing are marked with the symbol in the ICN.

 

Important:

• If a part from a VAA variant that has been saved via database (with active versioning) is changed in HiCAD, this change of the part will be lost as soon as the VAA is changed, and is updated accordingly when the drawing is opened.

Example:

• Draw a part, create a feature variant of it (VAA) and use the Part data synchronisation function to save it to the database.
• Then, create a new drawing file and insert the variant, via the database, in the drawing, e.g. with the Insert part, via DB article master function.
• Change the geometry of the variant, e.g. by applying a chamfer.
• Save the drawing and close it.
• Change the variant, e.g. with the Variant Editor.
• If you then re-open the drawing that you created beforehand, and the variant is updated accordingly, the chamfer will have disappeared.

To avoid this, i.e. to preserve the chamfer, you need to save the geometry to the variant. This means that after applying any geometry changes to a variant, it needs to be saved with the "Save to variant" function.

• If a part from a VAA variant that has been saved via database (with active versioning) is externally referenced after its insertion, the part will only be updated via external referencing (i.e. the .KRA file in RefTeile1) afterwards. This means that the updating via VAA will be "blocked" by the external referencing.

Create Feature Variant (3-D) • Variant Editor • Referencing Functions (3-D) • Variants - Example (3-D)