In-contexting problem

[rokahn]

When I insert a new empty part into an assembly using in-contexting, it remains underdefined. This seems contrary to the SW getting started manual on p14-13 where it says,

1 Click Insert, Component, New Part. Select a new part
from the Tutorial tab. Enter a name for the new
component, such as Pin.sldprt, and click Save.
2 Click the narrow model face on the front of the
assembly. The new part will be positioned on this
face, with its location fully defined by an InPlace
mate.

In my case, I'm using a series of offset planes in my assembly and I in-context the new part based on one of these planes. The part appears in the featureMgr in red with a (-) next to it, indicating that its location is not fully defined.

I've tried adding additional relations but I haven't yet figured out how to fully define the new part's location.

Note, at this point, the new part is empty but adding entities to the part sketch doesn't help either.

 

[meintsi]

The part may be mated to the plane, but is it still free to rotate?

Remember...
"If you don't use your head,
your going to have to use your feet."

 

[SBaugh]

This may not help your in-contexting problem but this may help you to understand in-contexting better!

In-contexting tips:

http://www.frontiernet.net/~mlombard/incontexttips.html

Also to view the thread that started all of this you can view it at comp.cad.solidworks If you have no way of getting there then check out these sites to get access to it:

Thread name is: Opinions on In-Context and InPlace Mates (Top-Down Design)

http://mechengineer.com/snug/

http://www.mailgate.org/comp/comp.cad.solidworks/

http://www.solidworks.com/html/contacts/getnewsgroup.cfm

http://www.google.com

I hope this helps you and everyone else that looks at this thread.

Best Regards, Scott Baugh, CSWP
credence69@REMOVEhotmail.com

http://www.3dmca.com

http://home.insightbb.com/~scott.baugh/

*When in doubt always check the help first*

 

[aart2]

Rokahn,
I think you do it right. The '-' sign in the feature manager means that you can collapse the part. When you click on the '-',it will change to a '+' sign. Try it.

So when this is it, you don't have a problem at all.

When you exit the edit-part-environment, check the in-context mate that SW has generated for your part. This is a 'Inplace' mate. When you suppress it you can move the part around anyway. But be careful! Don't do this when you have defined relations of your 'in-context'part to the other parts in the assembly, because this will have effect on the geometry of your 'in-context'part.
Hope this is useful for you,
Aart

 

[APPENG]

Rokahn,

I think aart2 is right, a lot of it depends on where the "-" sign is. The "-" sign that indicates the status of the part is indented and right before the part name and will be in between parenthesis, It will either say (-), (f), or (+). or else it will not appear at all.

In your feature manager you will see it like this...when the part features are collapsed:

Assembly1
|-Annotations
|+Lighting
|-Plane1
|-Plane2
|-PLane3
|-Origin
|+ <part symbol> (status) Part1 <instance ID> (Config Name)

When expanded you will see the minus sign in place of the + only to indicate that you can double click there to collapse the items under it (just like in windows explorer)

Assembly1
|-Annotations
|+Lighting
|-Plane1
|-Plane2
|-PLane3
|-Origin
|- <part symbol> (status) Part1 <instance ID> (Config Name)
|-Annotations
|+Lighting
|-Plane1
|-Plane2
|-PLane3
|-Origin


(-) means the part is free to move in some or all degrees of freedom
(f) means the component is fixed in space unable to move in any way.
(+) means that the part has mates that overdefine its location in the assembly.

If nothing appears, it means that the component has enough mates to fully define its location in space.

When Inserting a component via the INSERT/COMPONENT/NEW PART method, you will select a face that you wish to correspond to the FRONT plane to be oriented with. When the selection is completed, the part receives what is known as an &quot;IN-PLACE MATE&quot; and essentially becomes mated to the surface that you selected as if you stuck the part on there with glue. It can not rotate, or translate with respect to the rest of the assembly.

Does this help? Regards,
Jon
jgbena@yahoo.com