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Is it an assembly or a part? How do you do it?

Question asked by Christian Roth on Oct 7, 2013
Latest reply on Oct 8, 2013 by Deepak Gupta

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We have a situation here that I am sure is not all that unique.

Part A, is a common part that is used in many applications, but it also used as the raw component part in which machining is applied.

Part A + B Machining = Part AB

Part A + C Machining = Part AC

Part A + D Machining = Part AD

and so on..............

So how does everyone implement this in Solidworks? I see a couple of different ways, but the biggest challenge is to due with updates on Part A.

Option 1

Save As Copy of Component A, and apply changes. Now have new part AB.

If for some reason Part A changes, I know have to update part AB,AC,AD,AE........... manually.

Option 2

Create an assembly with Part A, called Part AB. Apply machining to assembly (Cut Revolve & Cut Extrude).

Decent option. Shows well in WPDM and reflects what in the ERP.

Option 3

Import Part A into Part AB (not as an assembly). Apply features (cut....) to imported part.

Similar to Option 2, but less visable in WPDM. More difficult to manage and oritentate the part.

I much prefer option B. But I was curious what everone else does?

No one else has this question

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Wayne Schafer Oct 7, 2013 3:49 PM
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I would do it with configurations. I would model part A and do different configs for AB, AC, AD, etc.
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Lenny Bucholz Oct 7, 2013 4:04 PM

As Wayne said configs work great for this.

There is also making a new part with part in part of the bodies and then you can just add the features to the version specific, that way there is no copy issues, if Part A changes so does the other part in part files and the new features don't go and change the originals.

I use this alot for machining parts at different states in the manufacturing process

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Christian Roth @ Lenny Bucholz on Oct 7, 2013 5:54 PM

Lenny, do you have an example of this or could you explain it further. I would be intrested in this feature.

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Lenny Bucholz @ Christian Roth on Oct 7, 2013 7:34 PM

so start a new part call it AB and save.

now go to the pull down from insert, find part, then go pick A, then do it again and pick B, you may have to move B to A or the other away around, but the move\copy works just like mating in an an assembly, then save.

next you can combine them together to make on body and add any features you need to make it its own file, remembering that if you modify the original A and B this new part will update to the changes you made in them.

Inserting a Part into Another Part

Use Insert Part to insert a base part into another part document.

When you insert a part into another part:

The part into which you insert it becomes a multibody part.
The part you insert becomes a solid body.
If the inserted part contains mate references, you can use them to position the inserted part. A Body-Move/Copy feature is added to the FeatureManager design tree. You can move and rotate the body after you place it.

To insert a part:

With a part document open, click Insert Part (Features toolbar) or Insert > Part.
Browse to a part document and click Open. The Insert Part PropertyManager appears.
Under Transfer, select any combination of items from the inserted part to be included in the derived part. You can include items such as custom properties, sketches, and model dimensions. All transferred elements of the inserted part are placed in folders under the inserted part in the FeatureManager design tree.
Under Locate Part, select Locate part with Move/Copy feature to define a location for the inserted part in the Locate Part PropertyManager.
Optionally, if you want to independently edit the features of the inserted part without affecting the original part, under Link, click Break link to original part. You can also break the link to the original part later by listing the derived part's external references and selecting Break All. Once you break the link to the original, you cannot restore it.
Click . After you insert a part, you can move, copy, rotate, or mate it using Move/Copy Bodies (Features toolbar).

To change the configuration of the inserted part:

Right-click the part and select List External Refs.
Select a configuration in Configuration Name, and click OK.
You can also control the configuration with a design table. See Base Parts in Configurations.

Move/Copy Body PropertyManager

In multibody parts, you can move, rotate, and copy solid and surface bodies, or place them using mates.

To access this PropertyManager, click Move/Copy Bodies (Features toolbar) or Insert > Features > Move/Copy.

Bodies to Move/Copy

	Solid and Surface or Graphics Body to Move/Copy	Select the bodies in the graphics area to move, copy, or rotate. The selected bodies move as a single entity. The bodies that are not selected are treated as fixed. A triad appears at the center of mass of the selected bodies.
	Copy	Select to copy bodies, and set a value for Number of Copies . Clear to move the bodies instead of copying them.
	Number of Copies

Translate

	Translation Reference	Sets the translation direction. Select an edge or vertex in the graphics area.
, ,	Delta X, Delta Y, Delta Z	Sets the values to reposition the bodies.
	Distance	Available when you select an edge for Translation Reference . Sets the translation distance. Type a negative number to switch the translation direction.
	To Vertex	Available when you select a vertex for Translation Reference . Select a second vertex. The bodies move to the second vertex.

Rotate

Set values or use the triad to rotate the bodies.

	Rotation Reference	Select an edge or a vertex in the graphics area to define the rotation axis.
, ,	X Rotation Origin, Y Rotation Origin, Z Rotation Origin	Set values for the coordinates of the rotation origin (the point that the bodies rotate about). The default values are the coordinates of the center of mass of the selected bodies.
, ,	X Rotation Angle, Y Rotation Angle, Z Rotation Angle	Set values for the angle around the X, Y, and Z axes.
	Angle	Available when you select an edge for Rotation Reference . Sets the value for the rotation angle.

Bodies to Move

Select Constraints to apply mates between bodies. Set the options in the panes below.

Solid and Surface or Graphics Body to Move/Copy

Select bodies in the graphics area to move when the mate is applied. The selected bodies move as a single entity. The bodies that are not selected are treated as fixed.

Mate Settings

Entities to mate

Select two entities (faces, edges, planes, etc.) to mate together.

Add

Click to add the mate after selecting a mate type and setting parameters below. Click Undo to clear selections.

Select a mate type.

All the mate types are always shown in the PropertyManager, but only the mates that are applicable to the current selections are available.

Coincident

Parallel

Perpendicular

Tangent

Concentric

Distance

Select, then set Distance. Select Flip Dimension to change the direction.

Angle

Select, then set Angle.

Mate Alignment

Select one of the following:

Aligned	Places the bodies so the normal or axis vectors for the selected faces point in the same direction.
Anti-Aligned	Places the bodies so the normal or axis vectors for the selected faces point in opposite directions.

Mates

The Mates box contains all the mates in the mate set (all the mates added while the PropertyManager is open). When there are multiple mates in the Mates box, you can select one to edit that mate.

In multibody parts, you can apply multiple sets of mates to the same body. Mates specified within different sets can conflict with each other. For example, you can apply a perpendicular mate between two faces in one set, and in a different set, apply a parallel mate between the same two faces.

Options

Show preview

When selected, a preview of a mate occurs when you make enough selections for a valid mate.

Combine Bodies

In a multibody part, you can combine multiple solid bodies to create a single-bodied part or another multibody part.

You can add or subtract bodies, or keep material that is common to the selected bodies.You can only combine bodies contained within one multibody part file. You cannot combine two separate parts. However, you can create a multibody part by using Insert Part to place one part into the other part file. Then you can use Combine on the multibody part.

It is strongly recommended that you do not use the Combine feature to combine weldment bodies. It is not always possible to calculate the cut list properties accurately for a body created using the combine feature.

In these examples, the multibody part contains two separate extruded bodies.

Add	Combines solids of all selected bodies to create a single body.
Subtract	Removes overlapping material from a selected main body.
Common	Removes all material except that which overlaps.

Contents

Combining Bodies - Add
In a multibody part, you can combine multiple bodies to create a single body.
Combining Bodies - Subtract
In a multibody part, you can subtract one or more bodies from another body.
Combining Bodies - Common
In a multibody part, you can create a body defined by the intersection of multiple bodies.
Combine PropertyManager
In the Combine PropertyManager, you specify which bodies in a multibody part to add, subtract, or overlap.

Parent topicManipulation of Features

Related concepts
Multibody Overview

Related tasks

Move/Copy Bodies

Delete Body

Related reference

Move/Copy Body PropertyManager

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Dustin Biber Oct 7, 2013 4:27 PM
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My preference is Option 2. For the exact reasons you state regarding pdm and ERP. It essentially reflects the real world process. Unless there is a compelling reason not to, I always default to constructing models in a manner to reflect the real world product structure and/or manufacturing process.
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Roland Schwarz Oct 7, 2013 5:56 PM
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Option 4: Insert --> Part
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Christian Roth Oct 7, 2013 7:37 PM
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Replies from Roland and Lenny fall under Option 3.
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- Deepak Gupta @ Christian Roth on Oct 8, 2013 1:06 AM
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  In order of preference:
  
  Option 2 (much easier and no external references)
  
  Option 3 (inserting part into part, gives more options other than assembly features but will give external references)
  
  Option 1 (using design table)
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Is it an assembly or a part? How do you do it?

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Attachments

Inserting a Part into Another Part

Move/Copy Body PropertyManager

Bodies to Move/Copy

Translate

Rotate

Bodies to Move

Mate Settings

Mates

Options

Combine Bodies

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