SIEMENS. Multi-body modeling. spse01537

Transcription

1 SIEMENS Multi-body modeling spse01537

2 Proprietary and restricted rights notice This software and related documentation are proprietary to Siemens Product Lifecycle Management Software Inc Siemens Product Lifecycle Management Software Inc. 2 Multi-body modeling spse01537

3 Contents Proprietary and restricted rights notice Introduction Multi-body modeling Multi-body modeling Sheet metal design bodies Add Body command Add a body Add Body dialog box Activate Part Body command Activate Assembly Body command Toggle Design/Construction Body command Toggle a solid body type Multi-bodies in PathFinder Rename a design or construction body Show Body Features command Show Body Name command Show All Design Body command Hide All Design Body command Activity: Multi-body modeling Activity: Multi-body modeling Open part file Add a body Develop edges for the sheet metal feature Create a contour flange Finish the sheet metal body Create a mirrored body Create a mirrored part body Mirror the part Summary Multi-body publishing Multi-body publish Multi-body Publish command Multi-body Publish dialog box Publish a multi-body part Manage published files Open a multi-body published file Rename a multi-body published file Find a missing multi-body published file spse01537 Multi-body modeling 3

4 Contents Update the link for an out-of-date published file Recreate a published multi-body part Activity: Multi-body publishing Activity: Multi-body publishing Open a multi-body file Publish the multi-body file Open the assembly file Summary Lesson review Lesson summary Multi-body modeling spse01537

5 Lesson 1: Introduction Welcome to Solid Edge self-paced training. This course is designed to educate you in the use of Solid Edge. The course is self-paced and contains instruction followed by activities. Start with the tutorials Self-paced training begins where tutorials end. Tutorials are the quickest way for you to become familiar with the basics of using Solid Edge. If you do not have any experience with Solid Edge, please start by working through the basic part modeling and editing tutorials before starting self-paced training. Tutorials Supported Browsers Windows: o Internet Explorer 8 or 9 o Firefox 12 or higher UNIX/Linux o Firefox 9.x or higher* Mac: Safari 5.x or higher Java Plug In Required for search The search engine requires version or higher of the Java Plug In installed to your browser. The plug-in is available (free) in the Java Runtime Environment (JRE) 6.0. If you need to install the JRE, or an equivalent Java environment, visit the Java download site at Adobe Flash Player required for videos and simulations To watch videos and simulations, you must have the Adobe Flash Player version 10 or later installed as a plug-in to your browser. You can download the Flash Player (free) at the Adobe Acrobat Reader Some portions of the help may be delivered as PDF which requires Adobe Acrobat Reader 7.0 or higher. You can download the reader (free) from Internet Explorer Caveats IE9 Compatibility View. The HTML deliverables are fully supported when launched with the protocol or the file:/// protocol. However, if you are viewing the files from a local installation e.g, D://,you may need to enable Compatibility View. In IE 9, do the following: spse01537 Multi-body modeling 1-1

6 Lesson Lesson 1: 1: Introduction Introduction 1. Choose Tools/Compatibility View Settings. 2. In the Compatibility View Settings dialog box, select the Display all websites in Compatibility View check box. *Firefox Caveats Firefox recommends that users update the latest version for security issues surrounding Java. They do not recommend using older versions of Firefox due to these issues. See: Most customers install and launch our deliverables via protocol which is fully supported. However, Firefox has a default security setting that prevents the help from launching correctly from a UNC path (file:///). To change this setting, you need to change the value of the security.fileuri.strict_origin_policy preference: o o o In the address bar, type about:config. In the Filter field, type security.fileuri, if the value of the security.fileuri.strict_origin_policy preference is set to true, set the value to false. (Double-clicked the value to toggle it.) Restart the browser. 1-2 Multi-body modeling spse01537

7 Lesson 2: Multi-body modeling spse01537 Multi-body modeling 2-1

8 Lesson Lesson 2: 2: Multi-body Multi-body modeling modeling Multi-body modeling Multi-body modeling is a design method which uses more than one solid design body in a single file. In multi-body modeling, you can design many separate models in the same space and according to the same set of rules. This modeling method provides the ability to model many components of an assembly as a single part or sheet metal file. When placing a multi-body part into an assembly, the resulting multiple bodies are represented as a single entry in Assembly PathFinder and on a bill of materials. An entire assembly could be represented as a single multi-body part. Sometimes the assembly is more important than the actual components that make up the assembly. In multi-body modeling, part and sheet metal files can contain multiple design bodies. Part and sheet metal files can contain part and/or sheet metal design bodies. Design bodies Can be a part or sheet metal model type Can contain both ordered and synchronous features A part design body can contain a single solid or disjoint solids Sheet metal design bodies do not support disjoint solids New design bodies share the existing material properties of the initial design body Construction body You can switch a design body to a construction body. Construction bodies display is turned off by default in an assembly or draft file. Construction bodies display with the construction color (purple). Construction bodies do not publish. Editing a multi-body file Only one design body can be active, all other bodies are inactive. You can only add or remove features on the active design body. When performing a synchronous move on a face of the active design body, the inactive synchronous design bodies also participate in move operations where Design Intent relationships are identified. If you do not want a design body to change, ground the design body. Dimensions can be placed between all design body faces. Active design body You can make the selected design body active using the Activate Part Body command. The environment shifts and displays the tool ribbon for the active body type. The active design body displays in the normal part colors. Inactive design bodies display with an opaque color. Note The inactive solid body face style opacity is set by the adjustable setting accessed in Solid Edge options View tab. If the option dim surrounding assemblies when in place activated is off, then the inactive body is shown in full opacity. If the option is on, then the inactive body is shown dimmed by percentage controlled by the slider. 2-2 Multi-body modeling spse01537

9 Multi-body modeling Sheet metal design bodies Sheet metal files support both part and sheet metal design bodies. All synchronous bodies are held together by geometric relationships and are considered to be one body in any synchronous editing of the file. Edits made to the active design body also appear in the other design bodies in the file. Adding sheet metal attributes You can add sheet metal attributes to a file by: Switching to the sheet metal environment Adding a new sheet metal body Once the sheet metal attributes are added to the file, they are maintained, even if no sheet metal bodies exist in the file. When you add a sheet metal body to a file, the sheet metal attribute variables are added to the variable table. If the file previously contained sheet metal bodies, those sheet metal variables are kept within the variable table. All sheet metal design bodies residing in the same file have the same set of attributes: Material Thickness Bend Radius Neutral Factor Bend Relief Parameter If you add a sheet metal design body to a part file, the Gage tab appears on the Material dialog box. All sheet metal design bodies share the same gage and bend properties within the same file. When you select the Apply to Model button on the Material dialog box, all sheet metal bodies in the file recompute to accept the new sheet metal parameters. For example, the following file contains two design bodies. If you change the material type and material thickness in the active body, spse01537 Multi-body modeling 2-3

10 Lesson Lesson 2: 2: Multi-body Multi-body modeling modeling these attributes change for the other design body in the file. Transforming sheet metal bodies You can import elements into Solid Edge and then convert them on a body by body basis with the following commands: Transform to Synchronous Sheet Metal Transform to Sheet Metal (ordered environment) When you use the Transform to Synchronous Sheet Metal command, the first transformed body in the file sets the default parameters of the material table. For example, create a rectangular protrusion that is 3 mm thick in a synchronous part. When you transform the solid body to synchronous sheet metal, it becomes a tab with a material thickness of 3 mm. Any subsequent synchronous transformations of sheet metal bodies use the material setting of 3 mm that was defined by the previous bodies. 2-4 Multi-body modeling spse01537

11 Multi-body modeling The Transform to Sheet Metal command converts the entire active body, and the transformed feature is added to the last position in the history tree. Moving to synchronous You can use the Move to Synchronous command to move the features for multiple bodies at once. If features for more than one design body are in the selected list of the PathFinder, the move to synchronous operation maintains the body identity. When you move multiple bodies to the synchronous environment, the resulting features are listed in a sequential order that represents the body as it is converted. Flattening multi-body files You can create flat patterns of a multi-body file that contains multiple sheet metal bodies. The file can contain only one flat pattern at a time. If you need to create more flat patterns, you can delete the existing flat pattern and then create another one. You can use the Multi-body Publish command to publish the individual design bodies to separate files. Switching between part and sheet metal You can create files that contain sheet metal bodies in either the Part or Sheet Metal environment. You can use the Switch to Part and Switch to Sheet Metal commands to switch between the environments. Switching from Part to Sheet Metal does not create sheet metal attributes for the active body. If you wish to attribute the active body, use the Transform to Synchronous Sheet Metal command. If there are no design bodies in the part file when you switch to sheet metal, the base modeling feature determines the initial body type in the sheet metal file. If the base feature type is sheet metal, sheet metal attributes are added and the body becomes a sheet metal body. If the base modeling type is part, then no sheet metal attributes are added and the body remains a part body. If the part file contains a design body when you switch to sheet metal, the active body defines the body type in the sheet metal file. spse01537 Multi-body modeling 2-5

12 Lesson Lesson 2: 2: Multi-body Multi-body modeling modeling Copying sheet metal bodies When you copy a synchronous sheet metal body, the sheet metal attributes are removed from the body. The copied sheet metal body behaves like a part copy until the attributes are restored. Copy workflows that result in this attribute removal behavior include: Manipulate a body or the face sets of a body with the Copy option selected Press Ctrl + C on a body or face sets of a body Note Even though the sheet metal attributes are removed during the copy, you can use the Transform to Synchronous Sheet Metal command to reestablish the plate-connector model for the body. Editing a multi-bodies file When editing sheet metal features, such as dimples or beads, on design bodies, the body containing the feature you are editing does not have to be active. You can edit any feature on any design body. When you select a synchronous element on either an active or inactive design body, the steering wheel is displayed and you can move the steering wheel into position relative to any body. You can edit common synchronous features on all bodies simultaneously. For example, if there are synchronous holes on multiple design bodies, the edit is applied to all of the holes. You can dynamically edit multiple ordered features from different design bodies simultaneously. 2-6 Multi-body modeling spse01537

13 Multi-body modeling Add Body command The Add Body command environments. is on the Home tab Solids group in both ordered and synchronous A new part or sheet metal file contains a single design body. In a file with a single design body, the Design Bodies collector does not appear in PathFinder. If you want to use the multi-body modeling method, use the Add Body command to create a multi-body file. You can use the Add Body command in a new file to assign a name to the initial design body. The default name for the initial solid body is Design Body_1. As you add solid bodies to a file, the Add Body dialog box contains the active design body name. spse01537 Multi-body modeling 2-7

14 Lesson Lesson 2: 2: Multi-body Multi-body modeling modeling Add a body 1. Open a new or existing file. The file can be a part or sheet metal file. 2. Choose the Home tab Solids group Add Body command. 3. On the Add Body dialog box, click the design body type (part or sheet metal) to add. 4. In the Added body name box, type a name or use the default name. 5. Click OK. 6. Construct a body. Note The solid body is not created unless you complete this step. 2-8 Multi-body modeling spse01537

15 Multi-body modeling Add Body dialog box Add Part body Specifies that the added design body is a part type. Add Sheet Metal body Specifies that the added design body is a sheet metal type. Initial body name Specifies the name of the initial design body. The default initial body name is Design Body_1. Added body name Specifies the name of the new design body. If you do not enter a name, the default name increments from the initial default design body name. spse01537 Multi-body modeling 2-9

16 Lesson Lesson 2: 2: Multi-body Multi-body modeling modeling Activate Part Body command You can only add or remove features on the active solid body. All inactive solid bodies are ignored during feature modeling. Use the Activate part body command to perform feature editing. Note to activate a solid body in order Even though you can only add or remove features from the active solid body, all solid body faces in the file participate in synchronous move operations. For example, you can: Right-click on a design body face and choose the Activate Body command. In PathFinder, right-click on a design body and choose the Activate Body command. In PathFinder, the active design body has an active body icon in front of the design body name Multi-body modeling spse01537

17 Multi-body modeling Activate Assembly Body command When you use a multi-body part in an assembly, you can control which design body of the multi-body part to apply assembly features to. You cannot apply assembly features to all design bodies of a multi-body part in a single operation. You specify which design body to apply assembly features to with the Activate Assembly Body command For example, you can:. The command is only available while in the part or sheet metal environment. Right-click on a design body face and choose the Activate Assembly Body command. In PathFinder, right-click on a design body and choose the Activate Assembly Body command. The icon in front of the design body in PathFinder denotes the active assembly design body. Note If you are in an assembly file, you can In-Place Activate the multi-body file to change the active assembly design body. If you attempt to delete the active assembly design body, an error message appears. Active Assembly Body: Assembly features require an Active Assembly Design Body. Do you want to delete the Active Assembly Design Body? OK to delete the Active Assembly Body and fail any downstream features. Cancel to return to modeling without deleting. If you attempt to toggle the active assembly design body to a construction body, an error message appears. Toggling to Construction will leave no active Assembly Body and may cause assembly features to fail. Do you still want to toggle to Construction? spse01537 Multi-body modeling 2-11

18 Lesson Lesson 2: 2: Multi-body Multi-body modeling modeling Toggle Design/Construction Body command In a multi-body part or sheet metal file, you can switch a solid body type to construction or design. When you switch a design body to a construction body, the construction body appears in the Construction Bodies collector. Note The toggle command only applies to solid bodies. Open volumes (detached bodies) cannot be toggled. The icon in front of the solid body in PathFinder denotes a construction body type Multi-body modeling spse01537

19 Multi-body modeling Toggle a solid body type In a single body file: 1. Open a file that contains a single solid body. 2. In PathFinder or in the model window, right-click on a solid body. 3. On the short cut menu, choose the Toggle Design/Construction command. Note If the solid body is a design body, the toggle makes it a construction body. If the solid body is a construction body, the toggle makes it a design body. In a multi-body file: 1. Open a file that contains more than one solid body. 2. In PathFinder, in the Design Bodies collector, right-click a design body. Note You can also right-click on the feature in PathFinder or right-click on a body in the model window. 3. On the short cut menu, choose the Toggle Design/Construction command. The design body becomes a construction body and is added to the Construction Bodies collector. Note These steps are the same if a construction body exists and you want to change it to a design body. spse01537 Multi-body modeling 2-13

20 Lesson Lesson 2: 2: Multi-body Multi-body modeling modeling Multi-bodies in PathFinder When more than one design body exists in a part or sheet metal file, PathFinder displays additional collectors. You use these collectors to manage design bodies. The main collector is named Design Bodies. All solid design bodies reside in this collector. When you change the design body type to construction, a Construction Bodies collector displays. You can turn the display on or off for any design or construction body. Design Bodies collector Construction Bodies collector Design body features Construction type features Active design body Inactive design body Active design body in assembly Active construction body Inactive construction body Groups and User Defined sets The creation of groups and user defined sets in PathFinder that include a design body is not supported. You can create groups and user defined sets that include features of design bodies Multi-body modeling spse01537

21 Multi-body modeling Rename a design or construction body 1. Open a file that contains more than one solid body. 2. In PathFinder, right-click a design or construction body and choose Rename. 3. Type in the new body name and press Return. spse01537 Multi-body modeling 2-15

22 Lesson Lesson 2: 2: Multi-body Multi-body modeling modeling Show Body Features command Use the Show Body Features command to highlight all features that are in a design or construction body. All features in the selected body display with green text in the Features collector in PathFinder. These features also highlight in the model window. You right-click on a design or construction body to display the command on the shortcut menu. Note This command selects all features in a design or construction body. If you want to select specific features in a design or construction body, select the features in the Features collector Multi-body modeling spse01537

23 Multi-body modeling Show Body Name command Use the Show body name command to append the design body name to the design body features in the Features collector. You select or clear this command. Show body name (Off) Protrusion2 Show body name (On) Design Body_1.Protrusion2 Note When you select the command and QuickPick finds a design body, the body name displays in the QuickPick list. spse01537 Multi-body modeling 2-17

24 Lesson Lesson 2: 2: Multi-body Multi-body modeling modeling Show All Design Body command Displays the design body. When you hide the design body for a part and then save and close the file, the design body will be hidden when you open the file later. If you save a preview with the design body hidden, the design body is not shown in the preview Multi-body modeling spse01537

25 Multi-body modeling Hide All Design Body command Hides the design body. When you hide the design body for a part and then save and close the file, the design body will be hidden when you open the file later. If you save a preview with the design body hidden, the design body is not shown in the preview. Hiding the design body can also make it more difficult to place the drawing views you want in a draft document. spse01537 Multi-body modeling 2-19

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27 Lesson 3: Activity: Multi-body modeling spse01537 Multi-body modeling 3-1

28 Lesson Lesson 3: 3: Activity: Activity: Multi-body Multi-body modeling modeling Activity: Multi-body modeling Create a sheet metal bracket (1) around an existing part (2). The bracket is a sheet metal body. When the bracket is complete, mirror the bracket to create an additional body. 3-2 Multi-body modeling spse01537

29 Activity: Multi-body modeling Open part file Open multi_body_a.par. spse01537 Multi-body modeling 3-3

30 Lesson Lesson 3: 3: Activity: Activity: Multi-body Multi-body modeling modeling Add a body On the Home tab Solids group, choose the Add Body command. On the Add Body dialog, click the Add Sheet Metal Body button (1). Type left bracket in the New body name: field (2). Click OK. 3-4 Multi-body modeling spse01537

31 Activity: Multi-body modeling Develop edges for the sheet metal feature A sheet metal contour flange feature requires edges. On the Sketching tab Draw group, choose the Project to Sketch command. Select the face shown for the sketch plane. On the Project to Sketch Options dialog, click OK. On command bar, use the Single Wireframe option. Select the six edges shown. Do not select the chamfer edges in the corners. On the Sketching tab Draw group, choose the Trim Corner command. Use this command to connect the six line segments. spse01537 Multi-body modeling 3-5

32 Lesson Lesson 3: 3: Activity: Activity: Multi-body Multi-body modeling modeling Create a contour flange On the Home tab Sheet Metal group, choose the Contour Flange command. On the Contour flange command bar, select the Single option. Select the five lines shown and then click the direction handle. Note Before selecting the first line, pause over the line and right-click to display QuickPick. Make sure you select the Edge (Sketch) entry. Click the arrow to create the flange outside the edges. In the dynamic edit box, type 60 for the distance and press Return. 3-6 Multi-body modeling spse01537

33 Activity: Multi-body modeling Hide all sketches. Notice in PathFinder that the sheet metal body (1) is in the Design Bodies collector. spse01537 Multi-body modeling 3-7

34 Lesson Lesson 3: 3: Activity: Activity: Multi-body Multi-body modeling modeling Finish the sheet metal body Add more flanges to complete the sheet metal bracket body. Click on the flange edge as shown. Press and hold the Ctrl key while selecting the additional flange edges shown. Click the handle shown. 3-8 Multi-body modeling spse01537

35 Activity: Multi-body modeling On the Flange command bar, click the Material Outside option (1). On the dynamic edit box, type 25 for the distance and press Return. Sheet metal body is complete. spse01537 Multi-body modeling 3-9

36 Lesson Lesson 3: 3: Activity: Activity: Multi-body Multi-body modeling modeling 3-10 Multi-body modeling spse01537

37 Activity: Multi-body modeling Create a mirrored body Create an additional bracket for the right side. In PathFinder, turn on the display of the reference plane named mirror plane. In PathFinder, select the design body named left bracket. On the Home tab Pattern group, choose the Mirror command. Select the mirror plane (1). Press the Esc key to end the command. Notice in PathFinder that the mirrored body is a construction body. The Sheet Metal environment does not support disjoint bodies, so the mirror operation automatically creates a construction body. In the Part environment, you can have a disjoint body. The mirror operation in the Part environment creates a disjoint body. The next portion of this activity covers the additional step required to create a mirrored body in the Part environment. In PathFinder, right-click on the construction body and choose the Toggle Design/Construction command. This places the body in the Design Bodies collector. Rename the body to right bracket. spse01537 Multi-body modeling 3-11

38 Lesson Lesson 3: 3: Activity: Activity: Multi-body Multi-body modeling modeling Create a mirrored part body The next portion of the activity covers how to create a mirrored part body. In PathFinder, turn off the display of the design bodies (1) left bracket and right bracket. Turn on the display of the design bodies (2) left plate. Right-click on body left_plate and choose the Activate Body command Multi-body modeling spse01537

39 Activity: Multi-body modeling Mirror the part In PathFinder, select the design body left_plate. On the Home tab Pattern group, choose the Mirror command. Select the mirror plane and then press Esc to end the command. Notice in PathFinder that no new body is created. The design body left_plate now consists of the original plate and a mirrored plate. This is a disjoint solid body. To create a separate body, we will detach the mirrored feature. In PathFinder, right-click on the mirror feature and choose the Detach command. The mirrored feature display turns off. The mirror feature in now a construction body. Right-click the new construction body and choose the Toggle Design/Construction command. Rename the new body to right_plate. spse01537 Multi-body modeling 3-13

40 Lesson Lesson 3: 3: Activity: Activity: Multi-body Multi-body modeling modeling This completes the activity. Save the file Multi-body modeling spse01537

41 Activity: Multi-body modeling Summary The multi-body file contains of five bodies. This multi-body file can be used as a single component in an assembly representing a single part number. You can also publish the multi-body file which creates five new files which contain a single body in each file. The image below is for illustration purposes only. In a multi-body file, only the activated body displays as shaded. All of the other bodies display as opaque. spse01537 Multi-body modeling 3-15

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43 Lesson 4: Multi-body publishing spse01537 Multi-body modeling 4-1

44 Lesson Lesson 4: 4: Multi-body Multi-body publishing publishing Multi-body publish In multi-body modeling, you may want to have each design body reside in an individual file. There are a number of reasons for this. Account for the design body as a unique part number in an assembly bill of materials Flatten a sheet metal model Reuse the individual model in another context Build an assembly from the multi-body part models Apply assembly features on all bodies Use the Multi-body Publish command to write each design body of a multi-body file into a separate file. The command also provides the option to create an assembly using the multi-body published parts. 4-2 Multi-body modeling spse01537

45 Multi-body publishing Multi-body Publish command Use the Multi-body Publish command to create an individual file for each design body in a multi-body file. All design bodies in the multi-body file are published. The command is only available if a file contains more than one design body. In the part environment, the command resides on the Home tab Solids group Add Body list. In the sheet metal environment, the command resides on the Home tab Sheet Metal group Add Body list. The command opens the Multi-body Publish dialog box. You use the dialog box to publish design bodies and also to manage the published files. The Multi-body Publish command also allows you to create an assembly file with the published bodies as components. spse01537 Multi-body modeling 4-3

46 Lesson Lesson 4: 4: Multi-body Multi-body publishing publishing Multi-body Publish dialog box Body column Lists the design bodies found in the multi-body file. Status column Displays a status icon for each published file. Each of the status icons are described in the Manage published files help topic. Filename column Lists the published files folder location or URL, and file name. Files managed by Solid Edge SP and Teamcenter do not display a path. The files are generated in the cache. Interaction with the Product Data Management (PDM) system determines the file names. Create Assembly Creates an assembly once the design bodies are published. Set Path Sets the file path on a first time publish and also when you perform a recreate. Note This option is not available in a Solid Edge SP or Teamcenter managed environment. Open Opens a published file when you right-click it and choose Open. Rename Renames a published file when you right-click it and choose Rename. Recreate Recreates a published file that is lost when you right-click it and choose Recreate. In the status column of the published file, a question mark denotes that a linked file cannot be found. Clicking the Save Files button publishes the file again and a linked symbol denotes link established. Find Finds a moved published file when you right-click it and choose Find. Save Files Publishes and saves the files. 4-4 Multi-body modeling spse01537

47 Multi-body publishing Publish a multi-body part 1. Open a part or sheet metal file which contains more than one design body. 2. Do one of the following: In the part environment, choose the Home tab Solids group Add Body list Multi-body Publish command. In the sheet metal environment, choose the Home tab Sheet Metal group Add Body list Multi-body Publish command. The Multi-Body Publish dialog box displays. Note In a Teamcenter managed environment, the owner is the CAD system, so the body name is written to the corresponding document s dataset name when you publish the documents. In Solid Edge SP, the body name is written to the title. 3. If you want to create an assembly file using the published file components, select the Create Assembly check box. 4. Click Save Files. 5. If you are working in a managed environment, update the property data in the Edit Profile (Insight) or New Document dialog box (Solid Edge SP or Teamcenter), and then click OK. The file name for each component is determined upon check in to the database. The file names are replaced by the Item ID in the Multi-Body Publish dialog box. 6. Click Close. spse01537 Multi-body modeling 4-5

48 Lesson Lesson 4: 4: Multi-body Multi-body publishing publishing Manage published files What is a Published file? A published file contains a part copy feature that links to the design body in a multi-body file. The published file is the same document type (part or sheet metal) as the design body in the multi-body file. Opening a published file You open a published from inside the Multi-body Publish dialog box by right-clicking on a filename and choose Open. You can also open a published file from Windows Explorer. Note Moving a published part copy feature from ordered to synchronous produces the following error Linked Part Copies detected. This action removes the link to the design body. Renaming a published file In the Multi-body Publish dialog box, right-click on a filename and choose Rename. What is an Out of Date published file? If you make a change to a design body that was published, the associated published file switches to an out-of-date status. The published file status displays in the Multi-body Publish dialog box. To update the file, right-click on the filename and choose Open. The published file opens and the Update Model Links dialog box appears. Check the appropriate option and save the published file. How do you resolve a missing published file? If you move a published file to a new location, the status switches to linked file cannot be found. In the Multi-body Publish dialog box, right-click on the filename and choose Find. Locate the file in the Select Part Copy dialog box. How do you recreate lost published files? If the any published files are lost, you can recreate them. The status of the published file displays as. Right-click on the published filename and choose Recreate. The status changes to. Click the Save Files button. The status changes to recreate, the status changes to. If any lost published files are not checked for to inform you of additional action needed. 4-6 Multi-body modeling spse01537

49 Multi-body publishing Open a multi-body published file 1. Open a published multi-body file. 2. Do one of the following: In the part environment, choose the Home tab Solids group Add Body list Multi-body Publish command. In the sheet metal environment, choose the Home tab Sheet Metal group Add Body list Multi-body Publish command. 3. Right-click the published file to open. You can also select other published files to open at the same time by using the Shift and Ctrl keys. 4. Choose Open. You can also double-click the file in the dialog box to open the file. Note You can also open a published file by double-clicking the file in Windows explorer. spse01537 Multi-body modeling 4-7

50 Lesson Lesson 4: 4: Multi-body Multi-body publishing publishing Rename a multi-body published file 1. Open a published multi-body part. 2. Click the Multi-body Publish command. 3. On the Multi-body Publish dialog box, right-click a published file and choose Rename. 4. Change the name. Note If you change the path, the path must already exist. 5. Press the Enter to key to make the change. Note If you select more than one published file to rename at once, you can only change the path using the Browse for Folder dialog box. 4-8 Multi-body modeling spse01537

51 Multi-body publishing Find a missing multi-body published file 1. To simulate a missing published file situation, move a published file to a new location. 2. Open the parent multi-body file. 3. Click the Multi-body Publish command. 4. On the Multi-body Publish dialog box, the moved published file displays a question mark denoting linked file cannot be found. Right-click the missing published file and choose Find. 5. Locate the published file in the Select Part Copy dialog box and click OK. 6. The Multi-body Publish dialog box updates showing a link status for the published file. spse01537 Multi-body modeling 4-9

52 Lesson Lesson 4: 4: Multi-body Multi-body publishing publishing Update the link for an out-of-date published file 1. Open a published multi-body part. 2. Make a change to a design body and save the file. 3. Click the Multi-body Publish command. 4. On the Multi-body Publish dialog box, notice that the published file for the design body that changed shows an out-of-date status. Right-click the out-of-date published file and choose Open. 5. The published file opens and the Update Model Links dialog box appears. Check the appropriate option and save the published file. 6. Save and close the published file. 7. The Multi-body Publish dialog box updates showing a link status for the published file Multi-body modeling spse01537

53 Multi-body publishing Recreate a published multi-body part 1. Open a published multi-body part. 2. Assume the published files get deleted to set up the need for a recreate. Delete all of the published files. 3. Click the Multi-body Publish command. 4. On the Multi-body Publish dialog box, notice that all of the published files have a question mark in the status column. This means that the linked files could not be found. Right-click each published filename and choose Recreate. You can also select all of the published files at one time and choose Recreate. 5. The status field changes to a dash. Click the Save Files button. Notice that each design body publishes again and the status changes to show a link symbol. spse01537 Multi-body modeling 4-11

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55 Lesson 5: Activity: Multi-body publishing spse01537 Multi-body modeling 5-1

56 Lesson Lesson 5: 5: Activity: Activity: Multi-body Multi-body publishing publishing Activity: Multi-body publishing This activity covers the process for publishing a multi-body file. Create an assembly file and add the published components. 5-2 Multi-body modeling spse01537

57 Activity: Multi-body publishing Open a multi-body file Open the multi-body file multi_body_b.par. spse01537 Multi-body modeling 5-3

58 Lesson Lesson 5: 5: Activity: Activity: Multi-body Multi-body publishing publishing Publish the multi-body file On the Home tab Solids group, choose the Multi-body Publish command (1). Shown below, the filename path (1) is set to be the same as where the multi-body file resides. You can click on a filename and then select the Set Path button (2) to edit the path. You can change all the file paths simultaneously by selecting the first filename, hold down the Shift key, and then click the last filename On the Multi-body Publish dialog, notice that the filename of the file to publish (3) takes on the same name as the body. You can change the name by double-clicking the filename and then entering the desired name. You can create an assembly file with the published files as components by selecting the Create Assembly option (4). Selecting the Create Assembly option enables the editing of the assembly file path and filename. Rename the filename Design Body_1.par to main_body.par. Change the file paths for all of parts to publish. You can use the Set Path option or you can manually edit each path. 5-4 Multi-body modeling spse01537

59 Activity: Multi-body publishing Click the Create Assembly option. You can change the path and filename if you desire. Click the Save Files button. As the files publish, each file status changes to a link symbol (5) to denote a successful publish. The published files are linked to the body in the multi-body file. Close the Multi-body Publish dialog. spse01537 Multi-body modeling 5-5

60 Lesson Lesson 5: 5: Activity: Activity: Multi-body Multi-body publishing publishing Open the assembly file Open the assembly created with the Multi-body Publish dialog. Observe that the published multi-body file comes into the assembly as an Assembly Copy with five published components. 5-6 Multi-body modeling spse01537

61 Activity: Multi-body publishing Summary When a multi-body file is published, each body publishes to a part or sheet metal part file. You can apply the file properties to each published file. The Multi-body dialog can create an assembly file that contains the published files in an assembly copy. Publishing a multi-body file provides a way for each body to be accounted for in a bill of materials. If the multi-body file can be considered a single part number, then it does not need to be published. spse01537 Multi-body modeling 5-7

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63 Lesson 6: Lesson review Answer the following questions: 1. Describe what multi-body modeling is? 2. What are the two types of solid bodies? 3. In multi-body modeling, can you have part and sheet metal features in the same file? 4. Can a multi-body file contain both synchronous and ordered features? 5. How do you switch between a design body and a construction body? 6. What does the Activate Design Body command do? 7. What does the Activate Assembly Body command do? 8. What is multi-body publishing used for? 9. What is a published file linked to? 10. When an assembly is created with the multi-body publish dialog, how is the multi-body file inserted in the assembly? spse01537 Multi-body modeling 6-1

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65 Lesson 7: Lesson summary Multi-body modeling is a design method where you can model several parts in the same design file. Each body can represent a part. You can model with both part and sheet metal features in the same file. You can use the boolean commands to union, subtract, split, or intersect bodies to form the intended body. spse01537 Multi-body modeling 7-1

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