By now, you have heard that Creo Parametric 1.0 has been released and is the next generation of PTC’s parametric mechanical design software. You may have also heard that the user interface has been redesigned to have the ribbon present in all modes. In this article, we will look beyond the interface and point out several interesting functions that you will want to try for yourself.
With the ribbon interface present throughout, you may feel some anxiety over finding your favorite features and commands.
Clicking the Command Search icon will open a search field and you can type in a portion of the feature you are looking for. The list is dynamic and will update as you type. When you see the command you are looking for, clicking it from the list will initiate the feature! This is a shortcut to the command that will prove very handy as you learn Creo Parametric 1.0.
When a new feature is created, you now get a solid preview instead of the yellow, lightweight preview from prior versions.
The new faces create by the feature are displayed with a nice orange color, so you can easily identify the active feature. Also, notice the references are displayed in green. This allows you to see exactly how the geometry will look before you complete the feature.
You can now choose to display your models using the Shading With Edges option. This will color hard edges and tangent edges in black, making it easier to discern each surface patch.
Also, when you hover your cursor over a feature, the feature will pre-highlight in a transparent green color. This is a huge improvement over highlighting the feature edges in red and will make it easier to identify the feature you want to select.
The Extrude feature has a new option to Add Taper to the sides of the extruded feature. This is the same as adding a Draft feature with the Sketching Plane as the Hinge. For Designers that model molded or cast parts, this can save time and reduce feature count.
The New Edit Capabilities
When a feature is edited, several interesting things happen:
- The active feature is highlighted in orange
- Dimensions and drag handles are displayed
- For sketched features, the profile is also shown
- Drag the handles to resize or reposition the feature. The intersection of the active feature with the rest of the model is constantly regenerated. Also, Creo does not “roll back” the model, so you are seeing the active feature intersected with features that follow it. This is similar to Dynamic Regen from prior releases, but with much improved performance.
- Drag the vertices of the sketch or the dimension arrow heads. When you drag a sketch vertex, you can move it “left/right” or “up/down”. However, if you drag the white arrowhead of a dimension, you can only resize the sketch in that direction.
- Select a dimension and enter a new value. If you know the precise size you need, entering the value is faster than dragging to that value.
- Select a different feature and keep on editing! This is a new paradigm you may need to get used to. Since the model is continuously regenerated, you can quickly edit many features using this technique.
These are the same capabilities you have when the Attached Preview is shown after initial creation or when in Edit Definition.
The Helical Sweep feature now has an Attached Preview. Also, you can use the dragging techniques discussed in the previous section to dynamically edit the shape of the sweep.
The Sweep Feature
The “regular” Sweep feature from prior versions has been combined with the Variable Section Sweep feature to provide very powerful function that can handle both modeling situations. This move will increase your modeling flexibility by providing your sweep features with an “upgrade path” if you need more powerful functionality such as additional controlling curves, Relations using the trajectory parameter or Datum Graphs.
Selecting Sketcher Reference “On The Fly”
Have you ever started sketching a profile and then realized you would like to snap the sketch to some underlying geometry? You can now add these references “on the fly” by holding the [CTRL] and [ALT] keys and selecting the edge, plane, vertex, etc.
This new technique is much faster than stopping your sketch, clicking Sketch > References, selecting the items you need and then returning to your sketch work.
The New 3D Dragger
The 3D Dragger is a new marker displayed on the component being assembled.
Several things you can do with the 3D Dragger are:
- Translate or Rotate the component. You can drag along any of the three straight arrows to translate in one direction, drag one of the “leaves” to translate within that plane, drag the ball in the center to translate freely or drag along any of the three rings to rotate about the axis with the same color. This is an alternative to using [CTRL]+[ALT]+RMB/MMB to reposition the component.
- The Dragger arrows and rings go from being colored to being gray as you add constraints. This indicates which degrees of freedom are locked in and which are still free. In Figure 15, only translation along the blue direction is left open. This makes it much easier to determine what constraints are missing as you work.
- Snapping - assign one constraint reference and drag the component. It will snap to valid references as you translate the model. This can be useful in cases where it is hard to select the desired surface.
Many useful functions have been added to the Right Mouse Popup menu eliminating the need to activate a ribbon tab to perform a task. For example, if the Layout tab is active, you can now select a dimension and move it or press RMB > Properties to configure it.
Hopefully, the 10 new capabilities in Creo Parametric 1.0 discussed in this article will get you started reviewing and working with this exciting new product. There are also hundreds of additional improvements that could not be covered in this short space that will prove beneficial to your organization. Please use the Comments below to inform us on the functions you find most interesting with Creo Parametric 1.0!