• When exporting a STEP solid to Creo Elements/Direct Modeling, be sure to select the SOLID output option. When exporting a set of surfaces, select the SHELL option to enable Creo Elements/Direct Modeling to import the STEP file together with the Creo Parametric supplied topological bounding information. The SURFACE option only provides geometric bounding information (AP203 CC2) which is not preferred by Creo Elements/Direct Modeling.

• In absolute accuracy mode, Creo Parametric keeps the same value at all times during design.

• In relative accuracy mode, Creo Parametric allows the accuracy to vary with the extent of the largest design element in the model. This means that large models might have a very coarse data representation — i.e. an accuracy value outside the accuracy range of Creo Elements/Direct Modeling.

• Absolute accuracy is the preferred mode for exporting to Creo Elements/Direct Modeling. This value is basically dimensionless in Creo Parametric. It can be either 0.0012 mm or 0.0012 inches, depending on the current unit selected by the user. The default unit is inches.

• When you import a Creo Parametric model whose dimensions are expressed in inches, the dimensions must be converted to millimeters in Creo Elements/Direct Modeling. This introduces a factor of 25.4 (1 inch = 25.4 mm). Change the units to millimeters in Creo Parametric before you export the STEP file to Creo Elements/Direct Modeling, ideally by fixing the size of the model.

• Experience shows that the best Creo Elements/Direct Modeling import results are attained if Creo Parametric's geometry check did not detect any flaws in the model prior to import.

• Creo Parametric includes a switch called intf3d_out_extend_surface which is turned on by default. This switch may lead to self-intersection of surfaces which are outside the visible face. If you encounter such behavior, you should first verify it using GATHER and UNTRIM and export the data with the switch turned off.

• You can design models in I-DEAS that have a coarse distance accuracy, which may result in inconsistent data when importing a model into Creo Elements/Direct Modeling.

• STEP benchmark tests show very good bi-directional data exchange with solid models using the currently released Unigraphics STEP processors.

• Surfaces: geometry-bounded versus topology-bounded (setting topology-bounded preferred by Creo Elements/Direct Modeling).

• Solids: geometry-bounded versus topology-bounded versus solid (setting solid-bounded preferred by Creo Elements/Direct Modeling).

• When you export, you can set a specific accuracy value for B-spline curve approximation.

• Unigraphics works with a general accuracy setting that is valid throughout the session and can be adjusted by the user. The smallest possible value is 1.0E-5 mm, giving a good overlap with Creo Elements/Direct Modeling's range of possible accuracy values.

• If the accuracy produced in Unigraphics is too low to export to Creo Elements/Direct Modeling or to match the agreed accuracy of a process, there are several ways to enhance the accuracy in Unigraphics prior to export:

◦ All faces of a solid can be re-grouped and re-sewn together according to a new accuracy. It is important however, that the collection of faces has no more associativity with the solid. Otherwise, re-sewing will take the solid's accuracy value.

◦ If low accuracy is a problem along variable radius blends, the accuracy may be enhanced prior to export by editing the variable radius blend tolerance of a specific VRB. The edited VRB tolerance takes precedence in STEP export.

• STEP benchmark tests showed good results for the bi-directional exchange of data from valid solid models within CATIA V4. The AP203(6) or AP214(2) solid model CATIA output modes are recommended for the best results when importing model data into Creo Elements/Direct Modeling.

• CATIA allows closure tolerance values of 0.1 mm and sometimes coarser, which might require surface repair in Creo Elements/Direct Modeling.

• Make sure a solid model is a SOLIDE in CATIA.