Pro/ENGINEER Wildfire 4.0 now provides the ability to populate Layers using a new command called “Activate”, to create concave and convex rounds over an entire part without the need to pre-select edges using Autorounds, and to create a Simple Hole with an option for a drill point at the bottom of the hole and a chamfer and/or counterbore at the top of the hole.
First we’ll look at Layers and the new “Activate” command:
After creating a layer, hold down the right mouse button and select ACTIVATE. The icon next to the active layer will appear as shown below.
Once in this mode, any features created in the model will be automatically placed on that layer without the need to individually select the specific features or create rules.
This works for axes, points, planes, coordinate systems, 3D notes, etc. It works especially well when creating annotation elements in a model in conjunction with model based definition.
If you are going to be creating a group of annotation elements specific to a feature either manually or by using the new “Create Driving Dimension AE” command, you can define and activate the layer and have all of that information automatically populated to that layer.
To verify layer content simply select the layer from the dialog box.
To deactivate a layer, simply select the layer to highlight, hold down the right mouse button and select “Deactivate.” New features created will no longer be added to that specific layer and will be subject to any layer rules and config option that have been defined.
Note: “ALL” states in the View Manager can now be set to include layer status.
Let’s move on to the new “Autoround” feature:
Do you work with castings or molded parts? Do you find that you spend a lot of time adding rounds to complex parts? Autorounds was created to save you time and simplify creation of multiple rounds. All of the rounds shown in the first Model Tree (below) can be replaced with a single Autoround feature as shown in the second Model Tree example (below).
Simply select the Insert pull down menu and browse down and select the Autoround command.
The Autoround dashboard will then appear. Check the boxes for concave or convex shaped rounds and also enter a value for the size of the rounds. You can choose separate values for the size of each type or use the Same option.
Other additional options can be defined in the pull up menus titled Scope, Exclude, Options and Properties. Under the Scope menu, you can specify whether to round all sharp edges that exist by selecting Solid Geometry (which is the default option) or choose to add limits by activating the Selected Edges option and then selecting specific edges. You can also choose to turn on or turn off, Convex Edges and Concave Edges.
When the Exclude pull up menu is selected you are provided with a means to add limits to the Solid Geometry scope by defining edges to be ignored by this operation.
When the Options pull up menu is selected, you can check the Create Group option. This will change the way the rounds are displayed in the Model Tree. Instead of a single entry for Autoround, you will see a group containing multiple rounds. Each of those rounds can contain individual round sets. The value for the radius in each of those sets can then be controlled independently as shown below.
Lastly, let’s look at the most basic of features the “Hole” and see what is new:
When creating a Standard Hole using UNC, U NF, ISO, etc. you have always had the option to add countersinks and counterbores, and can control the drill point. When using the Simple Hole you would be left with a flat bottom hole unless you used the sketch command which added additional steps to complete the process.
Simple Holes have been enhanced to include countersinks, counterbores and drill points. At the same time, Standard Holes have been enhanced to include tapered pipe threads.
When placing a Simple Hole, notice that the drag handles for the placement references appear green if they are not associated to a surface and become white once attached to a surface or edge.
In the dashboard, with the Simple Hole icon selected, there are now icons for both flat bottom and drill point shapes.
Select the Drill Hole icon and additional icons will appear to the right. You can select the icon to add a counterbore, a countersink, or both.
You can also specify whether the depth of the hole is measured to the shoulder of the cylinder or to the tip of the drill point.
By selecting the Shape pull up menu, you can view all of the dimensions associated with the hole including countersink diameter and angle, hole depth to Shoulder or Tip, and drill point angle.
The same capability exists for editing dimensions specific to counterbores. This also works if both countersink and counterbore are selected.
Another new capability is found under the Standard Hole. You now have the ability to create tapered pipe thread holes based on NPT, NPTF or ISO_7/1 standards.
After selecting the Standard Hole icon, select the Create Tapered Hole icon. You will be able to choose from a listing of hole tables specific to industry standard tapered threads. Look to the center of the dashboard for countersink and counterbore icons.
As always, selecting the Shape pull up menu will provide access to a 2D cross section cutaway of the hole as well as any modifiable dimensions.
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