I need to make an assembly of approx. 100-150 of the same part. I basically need a linear pattern, but I want each instance of the part to be rotated a certain amount. Is this possible? Does anyone have any good ideas about how to accomplish this? I think you could do this in Part mode by preforming a sweep with twist along path. Is there any similar operation in Assembly mode?
Thanks!
Not directly. But you can create a curve driven feature pattern in a part file. Put this part into your assembly and then use a Feature Driven Pattern in the assembly to pattern your components.
linear componant pattern puts all of the components in the same orientation. I believe you will need to look into feature driven patterns. this would require an additinal part (can be a virtual component) that has a pattern feature that has the spacing and orientaion you require.
can you do a quick mock up (say 3-5 parts) using mates to show what you wish to accomplish?
Make this parent pattern in part then use Feature driven pattern in assembly it will work as per parent feature (Pattern in part)
Jed,
Welcome to the forum.
Like everyone said you are best to go with the feature driven pattern.
But I do remember a thread some months back that was similar to this.
I will look to see if I can find it.
I could not find it. But it showed the posts patterned along a guard rail.
Another thought is you can create and move the parts and create a macro
to possibly do this.
Thanks for all the replies! I think I'll try the feature-driven pattern.
I've attached a short "stack" that I'm looking for. I did this by using "Copy with Mates", which would work, but would take a while. I was also hoping to make this first assembly a "master", so that I could make new assemblies with different (but similar) parts and be able to make the stack shorter or longer by simply changing the # of instances.
Jed,
Patterns are powerful, but they can be somewhat limited.
Here's a solution using a SolidWorks Add-in named Genus Designer.
The first picture is the knowledge diagram that describes the assembly to be built.
The second picture is the UI created from the knowledge.
The third picture is the assembly created using 100 parts.
You have stated that you would like to make new assembly with different but similar parts. With Designer, you can vary the type and dimensions of each part in addition to the quantity. The fact that it can do this without first creating a pre-built assembly means that it can easily handle the open-ended nature of your problem.
Nice part is that the diagram is all the programming you need to do.
- Tim
Thanks Tim! I will do a little research on Genius Designer and definitely check that out. It looks like it will do exactly what I want!
OK, I'm having trouble with the Curve Driven Pattern. I think that will get me close, but I still can't get the results I want. I want the center axis to stay in a straight line (like it would in linear pattern or coincident mate). Then I want a point on the OD to follow the curve driven pattern from my part. Anyone have any ideas? Check out the sample assembly that I attached to my last post. This is the result I'm looking for, but I would like to do it with a pattern if possible. Thanks.
Here is an example using your assembly. You could use equations in defining the helix to make it more user friendly.
Thanks Wayne. That is very close to what I'm looking for, but I would like the axis of each part to be colinear. The final result should be a cylinder with each part rotated a certain amount. I think the equation driven helix might be a good idea, if I can get it to work how I want it to.
Sorry, I did not look close enough at the assembly to notice the axises were not colinear. The only accurate way to do this might be using the API to "Copy with Mates".
I think you may be right. I don't have much API experience, but I'll figure something out.
Thanks for all the help!
Here is an example from the API help file.
This example shows how to copy components with mates in an assembly.
'----------------------------------------------------------------------------
' Preconditions:
' 1. Open:
' <SolidWorks_install_dir>\samples\tutorial\driveworksxpress\mobile gantry.SLDASM.
' 2. Observe Leg<1> and Leg<2> in the FeatureManager design tree.
'
' Postconditions:
' Leg<1> is replaced by a copy of Leg<2>: observe Leg<3> in the mobile gantry.
'
' NOTE: Because this assembly is used in a SolidWorks online tutorial,
' do not save any changes when you close it.
'----------------------------------------------------------------------------
Option Explicit
Sub main()
Dim SwApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swSelMgr As SldWorks.SelectionMgr
Dim blRepeat(2) As Boolean
Dim SelectedComps As Variant
Dim RepeatOptions As Variant
Dim MateRefs As Variant
Dim InpValues As Variant
Dim FlipValues As Variant
Dim swAssy As AssemblyDoc
Dim swItem As Object
Dim arrMateEntities(2) As Object
Dim arrCompsToCopy(0) As Object
Dim boolstatus As Boolean
Dim dValues(2) As Double
' Disable Visual Basic error on implicit Query Interface
On Error Resume Next
Set SwApp = Application.SldWorks
Set swModel = SwApp.ActiveDoc
Set swAssy = swModel
Set swSelMgr = swModel.SelectionManager
Set swModelDocExt = swModel.Extension
boolstatus = swModelDocExt.SelectByID2("Leg-1@mobile gantry", "COMPONENT", 0, 0, 0, False, 0, Nothing, 0)
swModel.EditDelete
swModel.ClearSelection2 True
boolstatus = swModelDocExt.SelectByID2("Leg-2@mobile gantry", "COMPONENT", 0, 0, 0, False, 0, Nothing, 0)
Set swItem = swSelMgr.GetSelectedObject6(1, -1)
Set arrCompsToCopy(0) = swItem
swModel.ClearSelection2 True
'Repeat all mates except the coincident mate with the Right End@Universal Beam-1; mate to Left End instead
Set arrMateEntities(0) = Nothing
Set arrMateEntities(1) = Nothing
boolstatus = swModelDocExt.SelectByID2("Left End@Universal Beam-1@mobile gantry", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
Set swItem = swSelMgr.GetSelectedObject6(1, -1)
Set arrMateEntities(2) = swItem
swModel.ClearSelection2 True
blRepeat(0) = True
blRepeat(1) = True
blRepeat(2) = False
SelectedComps = arrCompsToCopy
RepeatOptions = blRepeat
MateRefs = arrMateEntities
dValues(0) = 0#
dValues(1) = 0#
dValues(2) = 0#
InpValues = dValues
blRepeat(0) = False
blRepeat(1) = False
blRepeat(2) = False
FlipValues = blRepeat
swAssy.CopyWithMates SelectedComps, RepeatOptions, MateRefs, InpValues, FlipValues
End Sub
I got one to work in an assembly. Kinda. This method requires an additional part.
Here is the method:
You have an assembly pattern of a part at both linear and circular offsets!
Perfect Brian! That's exactly what I was trying to do. I even tried making a "dummy" part and used feature driven pattern, but I must have been doing something wrong. I started a whole new assembly and followed your steps and got exactly what I wanted. Thanks!
Sorry, I did not look close enough at the assembly to notice the axises were not colinear. The only accurate way to do this might be using the API to "Copy with Mates".