Solid Edge can read the following data types from NX files:

• solid bodies

• sheet bodies

• assembly structure, including occurrence names, occurrence color, and file names.

NX can read Solid Edge solid part models and assemblies.

Solid Edge will import all geometry from an NX file, even if the geometry is not visible in NX. This includes geometry that is not displayed in NX, such as objects that are hidden and objects on layers that have display turned off.

To make all geometry visible in NX so you can see what will be imported, follow these steps:

1. Open the part or assembly in NX.

2. On the Application menu, click Modeling.

3. On the Format menu, click Layer Setting.

4. On the Layers dialog box, select All Layers from the pull-down list.

5. Select all of the layers in the list.

6. Click the Selectable button and then click the APPLY button.

7. On the Edit menu, point to Blank and then click Unblank All of Part to unblank all parts.

8. For assemblies, change all reference sets to entire part.

9. Press Ctrl+F to fit the display.

This is the set of geometry that Solid Edge will read.

After you determine the geometry that will be transferred, you can count the number of NX bodies.

To do this in NX:

1. On the Information menu, click Object.

2. On the Class Selection dialog box, set the Filter Method to Type.

3. On the Select by Type dialog box, select Solid Body and click the OK button.

4. On the Class Selection dialog box, click the Select All button.

   You will see a count of the solid bodies at the bottom of the screen.

5. Repeat these steps for determining the number of sheet bodies in the file.

JT exported from Solid Edge can be imported into NX where it is real PMI. The following PMI object types are supported:

• Datum Feature Symbol (Datum Frame)

• Datum Target

• Simple Dimensions

• Surface Finish Symbol

NX assembly and part files both have the same extension (.PRT). Because of this, you need to be careful when opening NX files in Solid Edge. The steps are slightly different depending on the type of file you are opening.

1. On the File menu, click Open.

2. On the Open File dialog box, in the Files of Type box, set the document format to NX files (*.PRT).

3. Select the NX assembly file you want to open.

4. On the Open File dialog box, click Open.

5. On the New dialog box, select an assembly template and then click OK.

In most large assemblies, it is unlikely that all of the NX files reside in the same folder as the top-level assembly file. NX creates an external file, load_options.def, which resides in the same folder as the file being opened. The file contains the rules and folders where the NX component files are located and how they are attached to the NX assembly file.

Solid Edge uses a similar file during the import operation to locate the NX files. The search_opt.def file resides in the same folder as the NX assembly file being opened. It contains a list of search paths to use when opening the NX files. Solid Edge searches through the specified folder and any subfolders. For example, if you want to search the UG Assembly Test folder and all subfolders, the search_opt.def file should contain the entry:

s:\UG Assembly Test\..\

• Import the non-associative Parasolid data into Solid Edge.

• Use associative embedding to create a link between the NX file and Solid Edge model.

1. On the File menu, click Open.

2. On the Open File dialog box, in the Files of Type box, set the document format to NX files (*.PRT).

3. Select the NX part file you want to open.

4. On the Open File dialog box, click Open.

5. On the New dialog box, select a part template and then click OK.

1. On the File menu, click New.

2. On the New dialog box, select a part template and then click OK.

3. On the Insert menu, click Part Copy.

4. On the Select Part Copy dialog box, in the Files of Type box, set the document type to NX Part Document (*.PRT).

5. Select the file you want to insert and then click Open.

Solid Edge allows you to open NX files that contain multiple solid bodies. You can use either a Solid Edge assembly or part template when opening the NX file.

If you use a Solid Edge assembly template to open a NX file containing multiple solid bodies, you can use the Import Multiple Bodies as a Single Part File parameter, found in the PSXMT.ini file, to specify how the file is opened. If the parameter is set to On, which is the default value, a part file containing multiple construction bodies is created and added to the assembly. If the parameter is set to Off, an individual part file is created for each body contained in the .prt file. A subassembly is then created, to which the individual part files are added.

If you use a Solid Edge part template to open a NX file containing multiple bodies, the solid bodies from the NX file are copied into the Solid Edge file and added as body features. The default names of the features will be "BodyFeature_n" where n represents the feature number in the Solid Edge part.

If you use the Part Copy command to open a NX file containing multiple solid bodies, or a combination of solid bodies and construction elements, each body is copied as a separate part copy feature.

When opening the file through Part Copy, unlike traditional translators such as IGES or STEP, Solid Edge does not attempt to stitch surfaces or Boolean solids. All of the bodies in the NX file are shown as construction elements. None are specified as a base feature, but you can use the Make Base Feature command to convert one of the bodies to a base feature. The Make Base Feature command is on the shortcut menu for all construction surface features regardless of how the body is created. The command is not available if the construction surface is not a solid or if a base feature already exists.

When updating a part copy feature, the feature will fail if the corresponding body no longer exists in the NX file. Also, if you add new bodies to the NX file, they are not added to the Solid Edge file when you update the part copy features. If you want Solid Edge to recognize additions to the NX file, you must do a separate insert part copy operation.

Solid Edge determines the out-of-date status for the part copy features based on the NX file and not on the individual bodies. This means the link status will be the same for all part copies within a single NX file.

When opening updated NX files in Solid Edge, the Update Part Copies Dialog box displays.  This dialog box allows you to update out-of-date NX files. You do not have to update out-of-date files when opening them. If you like, you can go back and update them manually.

1. In Feature PathFinder, right-click on the link you want to update.

2. On the shortcut menu, click Update Link.

Solid Edge Embedded Client supports interaction with Teamcenter-managed NX documents. The common property dialog boxes in Solid Edge are populated with the NX document's property information from Teamcenter. Then when managed Solid Edge documents are saved, they are saved into the same Item Revision as the NX document.

When you open an NX managed assembly, Solid Edge queries the Teamcenter preference TC_NX_View_Type for product structure expansion and uses the view type specified. A Solid Edge structure saved to the same Item Revision as the NX assembly uses the view type specified by the SEEC_Default_View_Type preference. As a result, a single Item Revision can have all the BOM line properties for both Solid Edge and NX. In this case, the CAD system that last saved the assembly wrote the BOM causing the other CAD system's data to be out of date. Additionally a single Item Revision could have two separate view types where each CAD system's structure is managed uniquely. This option requires an advanced Structure Manager (formerly Product Structure Editor) license from Teamcenter.

You can open Solid Edge assembly, part, and sheet metal files in NX

1. In NX, on the File menu, click Open.

2. Change the Files of Type filter to .ASM, .PAR, or .PSM.

This assigns a NX part name to the Solid Edge part. For example, Part1.PAR becomes Part1.PRT. Because of this, you will not be able to open a Solid Edge part (.PAR) file if a NX (.PRT) file with the same name already exists.

The follow table lists versions of Solid Edge and NX along with the coinciding version of Parasolid for each.

• Open a Solid Edge document

• Save a document

• Opening and saving Solid Edge documents

• Help for AutoCAD Users

• Working with foreign data

• Insert Object command

• Open command

• Save As command