Use the surface editor to modify and recreate the mesh and surface parameters of a skin surface feature.
You must license and activate the Creo Elements/Direct Surfacing and Parametrics modules to use this command.
To modify a skin surface with the Surface Editor,
1. Select a Face in the viewport. If the face has no skin feature, click Yes when asked whether you wish to create a skin surface feature for the selected face.
2. (Optional) General options:
◦ Preview: Preview the surface according to the actual wire body (mesh) and surface parameters.
◦ Chk&Fix: Check and fix the part after a successful update of the new surface.
◦ Update: When turned on, the surface corresponding to the actual wire body (mesh) and the actual surface parameters is created and integrated into the given part. A surface feature holds the data of the new surface.
◦ Disconnect: Use this option to integrate surfaces no longer connected at surface borders.
◦ Redo Blends, Control, Sel Blend: Use these options to suppress affected blends before surface integration and recreate them afterward. When Disconnect is on, Creo Elements/Direct Modeling removes blends and will not recreate them after surface reintegration.
◦ Surface Analysis: Use the Surface Analysis tool to analyze the quality of the surfaces during editing.
3. (Optional) Adjust Skin Parameters, or save or replace a mesh (wire body):
◦ Inner Tol: Select the degree of tolerance (maximal error) of the skinned surface on the inner ribs (if there are any). The Inner Tol list contains various tolerance levels, including that of part accuracy (Part Acc). A larger inner tolerance normally results in smaller data size for the surface.
◦ Continuity: Choose an option to create a smooth connection between the boundary of the new surface and an existing surface.
▪ Position: Connection between surfaces is not smooth.
▪ Tangent: Connection between surfaces is smooth.
▪ Curvature: Connection between surfaces is smooth and reflections are reduced or eliminated. The mesh curves used for the operation need a curvature continuous connection to their adjacent faces. Otherwise, the Curvature Continuity option is disabled. For best results, specify one adjacent face (or two faces at opposite boundaries) to which a skin surface will be added.
◦ Optimization: Use the Optimization functionality to increase the surface quality of skinned surfaces. Use Preview and Surface Analysis to view and analyze the results of each optimization level.
▪ Off: No optimization. Off is the default for surfaces without a smooth connection to a neighbor surface and for surfaces that contain a degenerated surface (a singular point).
▪ Low: Moderate optimization. Low is the default for surfaces that have smooth connections to neighbor surfaces and for surfaces without a degenerated surface (a singular point). Low will be used in most cases.
▪ Medium: Use Medium if Low does not lead to a good result. The surface quality increases, but the Skinning operation will take longer and the resulting surface will contain more data.
▪ High: Only use High if the lower levels do not lead to a good result. The surface quality increases, but the Skinning operation will take longer and the resulting surface will contain more data.
◦ KeepWire: Save the wire body to a container below the given part. Creo Elements/Direct Modeling gives it the same name as the surface feature. Use this option to save a work in progress.
◦ ReplaceWire: Replace the existing mesh with another wire part. Only a suitable replacement can correctly update later.
4. (Optional) Add new 3D curves to the mesh in the Create Wire Elem section:
◦ Isoline:: Add isolines of the preview surface to the wire body by picking a point on the preview surface or a wire body edge.
5. (Optional) Use the Modify Wire Elem section to select and modify vertices and/or wire body edges.
Vertex/Edge: Select one or more vertices or edges. Depending on whether you make a single or multiple selection, and on the type of selected curve (line, circle, b-spline, etc.) Creo Elements/Direct Modeling displays the different possible modify operations (Modify Op's):
◦ Position: Position selected elements. If the selected elements lie in a plane, Creo Elements/Direct Modeling displays an additional workplane for direction selection. Creo Elements/Direct Modeling creates an adjustable, temporary relation set to find the proper solution (see step 6). Select a positioning method:
▪ Free: Move selected elements using the Position dialog.
▪ Planar: Move the plane's geometry using the position dialog. Selected elements remain coincident with the temporary workplane.
◦ Chg Rad:
Change the radius of a 3D circle or arc. Creo Elements/Direct Modeling creates an adjustable, temporary relation set to find the proper solution (see step 6). Select a method:
▪ Chg Fillet: Change the fillet radius.
▪ Keep Vertex: Change the radius of a circle or arc while keeping its vertices fixed.
▪ Keep Center: Change the radius of a circle or arc while keeping its center fixed.
▪ Keep Peak: Change the radius of a circle or arc while keeping its midpoint fixed.
▪ Keep Vert+Tng: Change the radius of the circle or arc while keeping its tangent and either its start vertex or its end vertex fixed.
◦ Mod Spline:
Change a 3D spline curve. Creo Elements/Direct Modeling creates an adjustable, temporary relation set to find the proper solution.
◦ Split Edge: Split the selected wire edge.
◦ Delete Edge: Delete selected wire edges.
◦ Convert Curve:
Convert selected wire edges to spline curves.
◦ Merge Edge: Merge wire vertices.
6. (Optional) Modify Wire Relation: Fine tune your surface edits by modifying the temporary relation set created during some of the modify operations above:
a. Select a Vertex/Edge. Creo Elements/Direct Modeling displays current relation settings.
b. Modify relation options:
▪ Vertex Relation: A vertex relation describes the situation around the vertex. It includes coincidence relations (Coi) to neighboring edges, and can contain relations to keep edges tangent (Tangent) and to keep edge tangents within a tangent plane (Tan Plane). A vertex can also be fixed (Fixed). You cannot remove an existing vertex relation because its coincidence property is always present and cannot be modified. You can adjust other vertex relation values. The relation name and label contains information about its current parameters.
▪ Edge Relation: An edge relation describes the situation around the edge. It includes coincidence relations (Coi) to intersecting edges, and can contain relations to keep edges rigid (Rigid), fixed (Fixed), or planar (Planar, applicable only for spline edges), and to keep tangency and curvature information of edges (Keep applicable for spline edges only). You can remove an existing edge relation if it has no coincidence relation to other edges and if no other value is specified. The relation name and label contains information about its current parameters.
▪ Face Relation: A face relation is a special relation used during a planar positioning operation. It has no relation label and cannot be modified.
• For the Modify Wire Element option, Creo Elements/Direct Modeling treats selected vertices and edges as fixed elements with respect to their new location or new geometry. Creo Elements/Direct Modeling modifies all surrounding elements according to the specified relations. Creo Elements/Direct Modeling uses the relation set to keep a wire part's existing properties without forcing certain properties (e.g., the relation set keeps the tangency between edges but does not force tangency between two edges).
• Creo Elements/Direct Modeling typically approximates intersection edges that are neither fixed nor rigid by spline curves before modifications.
• You can view all relations in the relation browser.
7. (Optional) Click Undo Last Wire Modification to undo your last mesh modification.
8. Click to complete the operation.
Limitations
• The default relations set created after you select an element selection is a good first choice for modifying the selected elements. Even for mesh changes that appear simple, the relation set may have no solution or only solutions in a certain (e.g., move) direction. Ifyou receive no feedback after making your selection, the relation set is likely too restrictive. You should modify it by adding or removing relations or by changing the selected elements.
• Creo Elements/Direct Modeling tries to automatically fix edges so that wires are only modified locally. When such a relation set has no solution after several dragging attempts, Creo Elements/Direct Modeling asks you whether these automatically fixed edges should be unfixed. After you've modified the relation set, Creo Elements/Direct Modeling turns off automatic unfixing.
• You can use the Surface Editor for surfaces without defined skin features: Creo Elements/Direct Modeling assigns default skin parameters and a default wire, similar to that created by the Mesh command, but with spline curves replaced by straight lines and circles when possible.
• The more edges your surface has, the more relations required for mesh modification. Creo Elements/Direct Modeling better solves relations sets of smaller mesh size. Reasonable feedback is also more likely when editing smaller meshes.
• During wire modification, Creo Elements/Direct Modeling does not check whether it can skin the mesh. The mesh must fulfill the same prerequisites requested by the skinning operation before correct surface creation becomes possible (otherwise previewing the surface also fails).
• The Surface Editor supports the
fixpoint concept for spline curves by a split and join approach: Spline curves with fixpoints are split at their fixpoints before the wire modification, such that each spline curve segment can be modified individually. If possible, spline curve splits at fixpoints are removed after the wire modification.
Modify Wire Relation: Fine tune your surface edits by modifying the temporary relation set created during some of the modify operations above:
to complete the operation.