Tag Archives: Multi_Bodies

Making your multibody Sheet Metal Parts work properly!

Do you work with multi body Sheet Metal?

But just one Flat Pattern in the feature manager instead of many.

Actual

Required

To fix it just make sure you have this setting on in SolidWorks.

1. In an open part, go to Tools > Options > Document Properties > Sheet Metal

2. Check the option “Create multiple flat patterns…. ” under Flat pattern options and hit OK

3. Rebuild your part to get the required result.

4. For future, you may set the option in your part templates.

Exploding a Multi-body part -2

Continued to my earlier post on exploding a multi body part, here is another example.  I have used a Weldment part for his example.

Example 2: Exploding a Weldment Part.

1. Click here to download the SW2011 part files used for this example.

2. Unzip and open up Weldment Part-2011 file.

3. Set the “3DSketch1″ to show. Right click or click on “3DSketch1″ and select show.

4. Also make sure sketches are set to show under View menu.

5. Go to Insert > Features and select Move/Copy Bodies

6. Select the two bodies as shown in the pic under bodies to move/copy.

7. Expand Translate (as we want to move out the body) and give 15mm as Delta Z value.

8. Click OK to close the close the command and apply the changes. The bodies have moved out by 15 mm in Z direction.

9. Restart Move/Copy Bodies command using step 5 or right click any where on the graphics area and select Recent Commands > Move/Copy Bodies. You’ll have to restart the command for further steps.

10. Select the side body as shown. Select the “3DSketch1″ line for direction and give -15 as the distance value.

11. Click OK to close the close the command and apply the changes. The body has moved out by 15 mm.

12. Select the two bodies as shown in the pic. Give -15mm as Delta X value.

13. Click OK to close the close the command and apply the changes. The bodies have moved out by 15 mm in X direction.

14. Select the side body as shown. Select the “3DSketch1″ line for direction and give -15 as the distance value.

15. Click OK to close the close the command and apply the changes. The body has moved out by 15 mm.

16. Select the two bodies as shown in the pic. Give -15mm as Delta Z value.

17. Click OK to close the close the command and apply the changes. The bodies have moved out by 15 mm in Z direction.

18. Select the side body as shown. Select the “3DSketch1″ line for direction and give 15 as the distance value.

19. Click OK to close the close the command and apply the changes. The body has moved out by 15 mm.

20. Select the two bodies as shown in the pic. Give 15mm as Delta X value.

21. Click OK to close the close the command and apply the changes. The bodies have moved out by 15 mm in X direction.

22. Select the side body as shown. Select the “3DSketch1″ line for direction and give 15 as the distance value.

23. Click OK to close the close the command and apply the changes. The body has moved out by 15 mm.

24. You may hide the “3DSketch1″ if required. Right click or click on “3DSketch1″ and select hide.

25. You may add two configurations one showing collapsed bodies where as other one showing exploded bodies.

26. Download the completed SW2011 part file here.

Exploding a Multi-body part -1

Many of us have been dealing with multi body parts and sometimes we need to show an exploded view similar to what we do in assembly to give a presentable picture of the parts or to show more details. Creating an exploded view in assembly is quite easy using the tool available. But are there any ways to replicate same in a multi body part.

Let’s explore the ways to do it:

Assembly Method: The easiest method is to convert the multi body part to assembly using this quick method : Assembly from Part – No mates required and then explode them using the exploded view tool.

Part Method:This particular method takes the advantage of move/copy bodies. Let’s discuss this method with some examples.

Example 1: Exploding a Multi Body Part.

1. Click here to download the SW2011 part file used for this example.

2. Unzip and open up Multi Body Part-2011 file.

3. Go to Insert > Features and select Move/Copy Bodies.

4. Select the “Side Plug” body (the blue colored) under bodies to move/copy.

5. Expand Translate (as we want to move out the body) and give40mm as Delta Z value. You may give direction or value for the move/copy if required for your parts.

6. Click OK to close the close the command and apply the changes. The “Side Plug” body has moved out by 40 mm in Z direction.

7. Restart Move/Copy Bodies command using step 3 or right click any where on the graphics area and select Recent Commands > Move/Copy Bodies.

8. Select the two “Round Plugs”.

9. Expand Translate and give 25mm as Delta Z value.

10. Click OK to close the close the command and apply the changes. The “Round Plugs” have moved out by 25 mm in Y direction.

11. You may add two configurations one showing collapsed bodies where as other showing exploded bodies.

12. Download the completed SW2011 part file here.

To be contd… Check Part 2 here

Detailing Multibody Part – 2

This is in continuation to my post “Detailing a Multibody Part -1” where we discussed detailing a multibody part in various ways. Now we take a step further and see what else can be done in detailing in multibody.

Say you have a multibody part, then you might need to show the BOM and ballooning as well to give more information to other person reading the drawing.

Not a big deal, you can insert the BOM and use the Balloon to set up the things.  But you may not the get desired results.

Now how to set the things right?

  1. Switch back to Part.
  2. Click on Weldment on Weldment toolbar or Insert > Weldments > Weldment.
  3. This will convert the part into a weldment and will add a cut list.
  4. RMB (right mouse button) meaning right-click on the cut list and select update. This will update the cut list.
  5. RMB on cut list item 1 and select “Properties”.
  6. You may see the “Material” property there. As I have already assigned “ABS PC” to the part, it is listed there.  If you need you can assigned different material to each body. For this, expand the cut list and right-click on the body. Select Material and then select the material you want to set. I have chosen “Plain Carbon Steel”.
  7. Go back to cut list item 1 properties (as in step 5)
  8. You can see the updated material property. Add a new property named “Description” and add value as Plate. You can add any value as per need.
  9. Switch to Cut list item 2 and also add the description property. We’ll not change the material here.
  10. Click “OK” at the bottom of the cut list properties window to close and apply the settings/changes.
  11. Save your file.
  12. Now switch to drawing mode and insert a view.
  13. Right click on view or sheet and select Tables > Weldment Cut list or Insert > Tables > Weldment Cut list.
  14. If you haven’t select a view, you will be prompted to select a view. To select, simple click on the view.
  15. Weldment cut list property manager will appear.
  16. Set the cut list template and choose any specific configuration if you need.
  17. Finally click on OK and place the cut list at the appropriate place or if you want to set the position use anchor.

Now time to play with balloons..

  1. RMB on view or sheet and select Annotations > Auto balloon or click on Auto Balloon on Annotation toolbar or Insert > Annotations > Auto Balloon.
  2. Click on the view if you haven’t selected a view.
  3. Set the balloons location and position them as required.
  4. Click OK to close the command.

All done now. You can have complete bodies on sheet 1 with BOM and Balloons similar to an assembly and have details drawings for bodies on other sheets in the same drawing using method as stated here.

Detailing a Multibody Part -1


Multibody Part. A part with separate bodies within the same part document

The tittle speaks up everything and I see many time people asking for it.  So here you go.

There can be several ways to detail out a multi body part.

Relative View method:

  1. Start a drawing and inert a view.
  2. Right click on the view and select Drawing Views > Relative View or click Relative View on the View toolbar or Insert > Drawing Views > Relative to Model.
  3. Make sure you have selected the view or you’ll be prompted to select a planar face of the model. To select, simple click on the view.
  4. The part will open up with Relative View property manager.
  5. Click on “Selected Bodies” and select the appropriate body you want to detail out.
  6. Select faces for Font and Right sides if you want to orient the views in different ways.
  7. Click OK to exit Relative View property manager and switch back to drawing mode.
  8. Place your view and any further views as required.
  9. Dimensions as required.

Assembly method:

Convert the multi body part to an assembly, then detail them as single part. Here is quick way to convert them in an assembly.Assembly from Part – No mates required

Reference Configuration and Bodies method:

  1. Start a new drawing.
  2. Right click on the sheet and select Drawing Views > Model View or click Model View on the View toolbar or Insert > Drawing Views > Model View.
  3. Click on browse and select the multi body part.
  4. You’ll be prompted to place the view but don’t click anywhere on the sheet. Click on “Select bodies” under Reference configuration. You mat change the configuration in case you have multiple configuration in that part.
  5. The part will open up with “Drawing View Bodies” property manager.
  6. Select the appropriate body you want to detail out.
  7. Click OK to exit Drawing View Bodies property manager and switch back to drawing mode.
  8. Select the view orientation as required.
  9. Place your view and any further views as required.
  10. Dimensions as required.

Assembly from Part – No mates required

So far you must have been creating your assemblies from parts using Bottom Up method in which you first design and model parts, then insert them into an assembly and use mates to position the parts. To change the parts, you must edit them individually. These changes are then seen in the assembly OR using Top Down method in which one or more features of a part are defined by something in an assembly, such as a layout sketch or the geometry of another part. The design intent (sizes of features, placement of components in the assembly, proximity to other parts, etc.) comes from the top (the assembly) and moves down (into the parts).

Now take a case of multi body part which you might need as an assembly. The option might be to save the individual body as separate part using “Insert into New part” option, insert them into a new assembly and use mates to position the parts.

STOP using this method and let’s talk of a different and simple method/option called “Create Assembly” which will help us to create an assembly directly from a multi body part without getting into hassles of using Bottom Up method, hence saving a lot of time.

  1. Open or create the multi body part. I have created a steel table with legs and a table top. 
  2. Expand the Cut list or Solid body folder by clicking on the + sign next to Cut list or Solid body folder (As I have weldment part used for describing the method, you’ll see only cut list is being used in next steps)
  3. You will see the bodies contained in the different folder based on their shapes and sizes. Their name is automatically driven through SolidWorks.
  4. Rename (if you wish or need) their name to something meaningful or something you can recognize easily.
  5. Now right click on the cut list and select save bodies.
  6. Next you’ll see Save Bodies property manager. Click on Auto-assign Names.
  7. The names which you have given in step 4 will be applied to the bodies here. Don’t worry about the order of the bodies.
  8. Now comes the important step. Click on Browse under “Create Assembly” in the same Save Bodies property manager. This will prompt you to create/save a new assembly.
  9. Key in the required assembly name and click on save.
  10. Finally click OK under Save Bodies property manager to execute the command of creating the assembly.
  11. Hurray, you have just made an assembly from a multi body part. The new assembly will open up or in case it don’t, you can always open it up from the location where you saved it.
  12. Now you can use this new assembly for other assembly operations like exploded view, BOM, etc.
  13. Also any changes done in the part will be reflected in the assembly.