Liste des fonctions et des pièces

Click the Features and parts icon on the right side of the Feature list to collapse the list entirely. Click the icon again to reopen the Feature list.

Visualize a model at the point of the rollback bar; all features listed beneath the rollback bar become temporarily suppressed. Select the rollback bar in the Feature List and drag up and down to roll-forward and roll-backward. You can also right-click on a feature in the list and select Roll to here for immediate and precise rollback. Right-click on the rollback bar and select Roll to end to return the rollback bar to the end of the Feature list.

Keyboard shortcuts

An alternative to dragging the rollback bar is by using Keyboard shortcuts. Select the rollback bar and click the up and down arrow keys (↑ ↓) to roll-forward and roll-backward one step at a time in the Feature List.

If you are a collaborator with view-only permission and you change the position of the rollback bar, you no longer will see real-time updates of any changes made to the rollback bar by another collaborator. To fix this, reload your browser.

Pour obtenir une ressource supplémentaire du Centre d'apprentissage, suivez le conseil de l'enseignant ici : Utilisation de la barre de reprise (compte Onshape requis).

Click a feature/sketch name in the list to supply a selection for a dialog (or make the selection in the graphics area). Selecting a part, surface, or curve in the part list cross-highlights features applied to or used to create the current selection. Selecting a face or part in the graphics area also cross-highlights associated features.

To reorder items, drag an item in the Feature list (or multiple items; just click to select additional items; they do not have to be contiguous in the Feature list) to parametrically reorder them.

Cross-highlighting does not apply to composite parts.

Le filtre et la barre de recherche vous permettent de filtrer votre recherche par nom, type, dossier ou pièce. Cliquez sur pour ouvrir un menu déroulant proposant différentes options de filtre :

Saisissez un nom ou un type partiel de pièce/de fonction pour afficher les pièces et les fonctions correspondantes. Utilisez une commande spéciale (préfixée par deux points :) pour une sélection plus poussée :

• :part chaîne de caractères - Affiche les corps correspondants par nom et les fonctions par corps qui affectent directement ces corps.
• :type chaîne de caractères - Affiche les fonctions et les corps avec le type correspondant
• :name chaîne de caractères - Affiche les fonctions et les corps avec le nom correspondant
• :errors chaîne de caractères - Affiche les fonctions et les corps contenant des erreurs
• :folder chaîne de caractères - Affiche les dossiers d’ateliers de pièces avec le nom correspondant
• :variable chaîne de caractères - Affiche les fonctionnalités qui utilisent ou modifient une variable (distinction majuscules/minuscules)
• :suppressed chaîne de caractères - Affiche les fonctions supprimées
• :hidden chaîne de caractères - Affiche les fonctions et les corps cachés
• :shown chaîne de caractères - Affiche les fonctions et les corps non cachés

Par exemple, :part pièce 1 affichera la pièce 1, la pièce 10, la pièce 11, la pièce 12, etc., ainsi que tous les corps directement associés.

• Rename features - Right-click the name in the Feature list, and select Rename to edit the Feature name directly in the Feature list without opening the dialog.
• Suppress a feature - Use the Suppress command from the context menu of a feature to visualize the model without that feature
• Hide or show features - Use the Hide/Show command from the context menu of a feature to hide that entity from the graphics area view (or show it); you can also hover next to the name and click the icon.
• Show dependencies - Use the Show dependencies command from the context menu of a feature to open a dialog indicating the parents (above the up arrow) and children (below the down arrow) of the selected feature. Hovering over each arrow shows a tooltip indicating the feature relationship.

  

• Group sketches, features, and planes into folders - Select the items you wish to group together in the Features list, then right-click and select Add selection to folder... A Folder name dialog appears in which to enter a name for the folder. The name of the folder appears in the Features list, with an arrow to expand the folder to see the contents.
  • You can right-click on just the folder (with no other selections made) and select Unpack folder to remove the folder and return the items to being listed singly in the Features list.
  • Select Suppress to visualize the model without the selected folder of items. When a feature or folder is suppressed, all features associated with the suppressed item become inactive.
  • You can also make a selection and then click the folder icon at the top of the Features list .

    

    Effectuez la sélection des éléments à regrouper ; cliquez avec le bouton droit et sélectionnez Ajouter des sélections au dossier..., spécifiez un nom pour le dossier ; cliquez sur la coche

    

    Le dossier apparaît dans la Liste des fonctions ; développez pour afficher le contenu

    You can create nested folders by creating a new folder while inside an existing one.

Hover over the Parts, Composite parts, Curves, Meshes, or Surfaces title in the Parts list to see the icon. Click the icon to hide all entities in that list, click again to show all entities.

When an entity is hidden, hover over it in the list to see the outline of the entity appear in the graphics area.

In the Parts list, use the context menu (RMB) to access commands for the parts, surfaces, and curves, including but not limited to:

• Rename - Enter a new name for the item.
• Properties - Edit metadata for the item.
• Assign material - Use the Onshape material library or a custom library (if available) to assign a material (and therefore density) to the item.
• Edit appearance - Change the color of the item.
• Copy - Make a copy of the item in order to paste it somewhere else.
• Create drawing - Create an Onshape drawing of the selected item.
• Export - Opens the Export dialog, where you can export (download) the currently selected parts into a file (or individual files) on your device. See Exporting files for more information.
• Release - Create a Release candidate and begin the release process for the selected item.
• Release all configurations - For users who have the ability to create release packages, this command opens the Release candidate dialog with all configurations pre-loaded into the release package (up to 100 configurations are supported). This option is only available for configurations with a single List input. The command option is not available if there are multiple List inputs, or if Checkbox or Configuration variable inputs are used. You can always add configurations into the release package once the dialog is open (after clicking the Release command from the context menu).
• Revision history - Display the revision history of the selected item. If there is no revision history, a message is displayed.
• Hide - Hide the item from view.
• Hide other - Hide items other than the one selected.
• Hide all - Hide all items, including the one selected.
• Isolate - Make other items muted in color and unavailable for selection with the ability to expand opacity by either distance to the selected item or by connectivity to the selected item.
• Make transparent - Make the selected item transparent.
• Add comment - Add a comment and tag the selected item in the comment.
• Zoom to selection - Zoom the window so that the entire item is visible and centered in the graphics area, such that the largest possible view of the item is created.
• Delete - Discard the selected item.

Pausing regeneration

Clicking the Pause regeneration button () prevents Onshape from regenerating parts while editing. This can be useful when working with configuration tables or Part Studios that take a long time to regenerate. When regeneration is paused, you can make changes to tables, configuration tables, and quantities and booleans (non-selection fields), and regenerate the parts once editing is complete.

Paused regeneration mode limits many Onshape operations and should only be used when necessary. The primary use case for pausing regeneration is for modifying existing parameter values in batches.

To pause regeneration:

1. Click Pause regeneration () in the Features List.

   

2. With the Paused regeneration banner showing, make your edits.

   

3. Choose an option for applying or rejecting your changes:
   • To apply your changes and regenerate the Part Studio while still in Paused regeneration mode, click Regenerate Part Studio.

     

   • To apply your changes, regenerate the Part Studio, and exit Paused regeneration mode, click Regenerate features and exit.

     

   • To discard your changes and exit Paused regeneration mode, click Discard unregenerated changes and exit. Note that any changes applied with the Regenerate Part Studio button will be maintained when you exit; only changes that have not been regenerated are discarded.

     

   • To undo your discard and return to Paused regeneration mode, click Restore.

     

Tips

• Switching tabs or closing the document while in Paused regeneration mode will automatically apply the changes.

• Regenerated changes cannot be undone once the green checkmark is selected. To undo these changes, exit Paused regeneration mode and restore the document to a previous version.
• Sketches cannot be edited when regeneration is paused.
• La géométrie et les tables ne seront pas cohérentes lorsque la regénération est suspendue et seront mises à jour lorsque vous aurez terminé la regénération.
• Le mode de regénération suspendue n'est pas disponible en mode Réparation et vice versa.

Showing regeneration times

Clicking the Show regeneration times button () opens a display of all features and the time each takes to regenerate. You can use this to estimate which time-costly features to suppress to maximize modeling time without regenerating features you don’t need at the moment.

Passez la souris sur une fonction pour voir la mise en surbrillance correspondante sur le modèle (indiquée par les flèches bleues ci-dessus). Utilisez le menu Contenu de la Liste des fonctions pour supprimer une fonction spécifique.

If there are errors in the Feature list, the icon is shown in the upper left corner of the list. To filter by errors on the Feature list, click on this icon. Hover your cursor over the icon to see the number of errors:

Lorsque des sélections sont manquantes dans une fonction, le triangle jaune apparaît sur celle-ci. Passez la souris pour voir le nombre de sélections manquantes :

Lorsqu'une fonction n'est pas entièrement définie, l'indicateur bleu apparaît au-dessus de la fonction :