I am green at this.  The books do not give a good procedure.
Can someone put down the step by step method to create an in context
piece of hardware, i.e. a bolt in a hole in an assembly.
This would be greatly appreciated by a new SW user.  Thank you in
advance.

To put it simply, if you have an assembly open and are in Edit Part
mode, if you create a relationship to a different part in the
assembly, you have now created an in-context piece.

Any of the normal sketch relations - coincident, concentric, convert
edges (my favorite), etc. that are used with a piece of geometry in
another part creates an external relationship (another name for in-
context).

Another method is when you create Extrudes, Cut-Extrudes, etc. where
you use Up to Surface, Vertex, Offset from Surface etc. where the
surface is from another part in the assembly creates an external
reference.

The main issue you need to be aware of is that these external
relationships can only be updated in-context of the assembly where
they were created. You HAVE TO HAVE the assembly open if you want to
see these relationships work properly. These parts should also not be
used in more than 1 assembly - which lends itself great towards one-
off parts.

There's a good rule of thumb list on Matt Lombard's web site:
http://mysite.verizon.net/mjlombard/ Click on Rules of Thumb and then
select In-context relationships.

Good luck,

Steve O

On Feb 11, 1:20 pm, "SteveO" <ste...@tpm.com> wrote:
> To put it simply, if you have an assembly open and are in Edit Part
> mode, if you create a relationship to a different part in the
> assembly, you have now created an in-context piece.
>
> Any of the normal sketch relations - coincident, concentric, convert
> edges (my favorite), etc. that are used with a piece of geometry in
> another part creates an external relationship (another name for in-
> context).
>
> Another method is when you create Extrudes, Cut-Extrudes, etc. where
> you use Up to Surface, Vertex, Offset from Surface etc. where the
> surface is from another part in the assembly creates an external
> reference.
>
> The main issue you need to be aware of is that these external
> relationships can only be updated in-context of the assembly where
> they were created. You HAVE TO HAVE the assembly open if you want to
> see these relationships work properly. These parts should also not be
> used in more than 1 assembly - which lends itself great towards one-
> off parts.
>
> There's a good rule of thumb list on Matt Lombard's web site:http://mysite.verizon.net/mjlombard/Click on Rules of Thumb and then
> select In-context relationships.
>
> Good luck,
>
> Steve O

A guy at work told me that I could make an "in context" relationship
between a bolt and a hole in an assembly. Then I could populate an
assembly dwg with that bolt into every hole of that size in the
assembly. A very big time saver (dont have to mate each bolt to each
hole).  Is this the same thing you are saying?
If I mate a bolt to a hole in an assembly, i.e. an in-context mate,
then if bring another bolt into the assembly, it will automatically
locate itself in each of the same type of hole?  Do I have that
correct.  THANKS MUCH FOR THE HELP!

First, a simple mate does not create an in-context relationship. These
occur at the part Sketch and Feature level, not assembly mate level.

You're looking for a Feature Driven Pattern in the assembly. Use one
part with a series of holes either using the Hole Wizard or a linear/
circular pattern and then place your fastener set in the first hole.
then you can use the Feature Driven Pattern in the assembly to
populate the rest of the holes. No extra mates are created. This is
one of my favorite assembly tools.

Steve O

>> Steve O
>
> A guy at work told me that I could make an "in context" relationship
> between a bolt and a hole in an assembly. Then I could populate an
> assembly dwg with that bolt into every hole of that size in the
> assembly. A very big time saver (dont have to mate each bolt to each
> hole).  Is this the same thing you are saying?
> If I mate a bolt to a hole in an assembly, i.e. an in-context mate,
> then if bring another bolt into the assembly, it will automatically
> locate itself in each of the same type of hole?  Do I have that
> correct.  THANKS MUCH FOR THE HELP!
>

Also take a look in SolidWorks Help for "Smart Fasteners" and "Smart 
Fasteners Hardware Stacks"

John Layne
www.solidengineering.co.nz

> Also take a look in SolidWorks Help for "Smart Fasteners" and "Smart
> Fasteners Hardware Stacks"
>
> John Laynewww.solidengineering.co.nz

Doooh - Forgot all about that. Smart Fasteners should do a good job
for hardware.

Steve O

Something that you need to be careful of is if an element in a sketch
is "attached" or "linked" to the assembly or just initially
referenced.  As an example.  If a hole location is referenced from
Part A onto Part B and if the part A is moved later in the assembly
the hole in part B will move accordingly- sometimes causing real
problems.  Sometimes this can be helpful but for the most part this
can turn out to be a disaster.

One approach is to remove the reference constraint in the sketch.  The
edge or center then needs to be dimensioned or anchored etc.  Another
approach is to be sure that the "No External Reference" is toggled
on.  When No External Reference is on, no reference will be created
and the hole will not move when Part A is moved in the assembly.  This
is usually handy because once the hole is located in part B, part A
can then be constrained to the hole, just as the real fastener would
constrain the two parts together.

Hope this helps,

EdT

On Feb 12, 4:42 am, "Ed" <ed.thomp...@verizon.net> wrote:
> Something that you need to be careful of is if an element in a sketch
> is "attached" or "linked" to the assembly or just initially
> referenced.  As an example.  If a hole location is referenced from
> Part A onto Part B and if the part A is moved later in the assembly
> the hole in part B will move accordingly- sometimes causing real
> problems.  Sometimes this can be helpful but for the most part this
> can turn out to be a disaster.
>
> One approach is to remove the reference constraint in the sketch.  The
> edge or center then needs to be dimensioned or anchored etc.  Another
> approach is to be sure that the "No External Reference" is toggled
> on.  When No External Reference is on, no reference will be created
> and the hole will not move when Part A is moved in the assembly.  This
> is usually handy because once the hole is located in part B, part A
> can then be constrained to the hole, just as the real fastener would
> constrain the two parts together.
>
> Hope this helps,
>
> EdT

EdT,

where is the "No External Reference" located?

Ed wrote:
> Something that you need to be careful of is if an element in a sketch
> is "attached" or "linked" to the assembly or just initially
> referenced.  As an example.  If a hole location is referenced from
> Part A onto Part B and if the part A is moved later in the assembly
> the hole in part B will move accordingly- sometimes causing real
> problems.  Sometimes this can be helpful but for the most part this
> can turn out to be a disaster.
> 
> One approach is to remove the reference constraint in the sketch.  The
> edge or center then needs to be dimensioned or anchored etc.  Another
> approach is to be sure that the "No External Reference" is toggled
> on.  When No External Reference is on, no reference will be created
> and the hole will not move when Part A is moved in the assembly.  This
> is usually handy because once the hole is located in part B, part A
> can then be constrained to the hole, just as the real fastener would
> constrain the two parts together.
> 
> Hope this helps,
> 
> EdT
> 
Turning OFF External References IS NOT A SMART MOVE. Once you figure out 
how to utilize external references will save you time 99% of the time. 
Why in the world do you use a parametric based modeler if you don't use 
the power of it. You might as well be using a program like Cadkey or 
Autocad. True, external relations may cause problems in the beginning 
with circular references but once you understand them, it is a HUGE time 
saver. If I move a tapped hole or thru hole that has a mating hole, why 
have to make the same sketch edit in all the parts that this hole 
affects. Changing one dimension to update 3 or 4 other parts is worth 
the "disaster" that could happen if you miss one of those holes that was 
supposed to move. This is almost as helpfull as the good old autocrap 
days of manually editing a dimension rather than moving the geometry to 
where it is supposed to be and then giving that file to the CNC 
programmer to use for machining.

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j wrote:
> Ed wrote:
>> Something that you need to be careful of is if an element in a sketch
>> is "attached" or "linked" to the assembly or just initially
>> referenced.  As an example.  If a hole location is referenced from
>> Part A onto Part B and if the part A is moved later in the assembly
>> the hole in part B will move accordingly- sometimes causing real
>> problems.  Sometimes this can be helpful but for the most part this
>> can turn out to be a disaster.
>>
>> One approach is to remove the reference constraint in the sketch.  The
>> edge or center then needs to be dimensioned or anchored etc.  Another
>> approach is to be sure that the "No External Reference" is toggled
>> on.  When No External Reference is on, no reference will be created
>> and the hole will not move when Part A is moved in the assembly.  This
>> is usually handy because once the hole is located in part B, part A
>> can then be constrained to the hole, just as the real fastener would
>> constrain the two parts together.
>>
>> Hope this helps,
>>
>> EdT
>>
> Turning OFF External References IS NOT A SMART MOVE. Once you figure out 
> how to utilize external references will save you time 99% of the time. 
> Why in the world do you use a parametric based modeler if you don't use 
> the power of it. You might as well be using a program like Cadkey or 
> Autocad. True, external relations may cause problems in the beginning 
> with circular references but once you understand them, it is a HUGE time 
> saver. If I move a tapped hole or thru hole that has a mating hole, why 
> have to make the same sketch edit in all the parts that this hole 
> affects. Changing one dimension to update 3 or 4 other parts is worth 
> the "disaster" that could happen if you miss one of those holes that was 
> supposed to move. This is almost as helpfull as the good old autocrap 
> days of manually editing a dimension rather than moving the geometry to 
> where it is supposed to be and then giving that file to the CNC 
> programmer to use for machining.
> 
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> News==----
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> Newsgroups
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One additional bit of info using external references. If  you design 
tools or machines or whatever that are similar except for certain parts 
or sizes, external references are a HUGE time saver. We design tools 
that gage different sized airfoils and have one gage that we designed 
that took about 45-50 hours to do in Cadkey which is basically what 
you'd have if you turned of external references. This same tool is down 
to about 8 hours of total design time and we still get the same price 
for the tool at the 45 hour time which is about 1850.00 per tool and we 
do approx 20 of these every year and this is just one of the tools we 
design.

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> Turning OFF External References IS NOT A SMART MOVE. Once you figure out
> how to utilize external references will save you time 99% of the time.

Given the nature of the origional question, External References can
really cause problems with someone that is new.

> Why in the world do you use a parametric based modeler if you don't use
> the power of it. You might as well be using a program like Cadkey or
> Autocad.

Autocad is not really a 3D program and Cadkey is obsolete, Keycreator
is probably not a good investment.  Many would say that SW is the best
3D design tool but not every project benefits from parametrics.

>True, external relations may cause problems in the beginning
> with circular references but once you understand them, it is a HUGE time
> saver. If I move a tapped hole or thru hole that has a mating hole, why
> have to make the same sketch edit in all the parts that this hole
> affects. Changing one dimension to update 3 or 4 other parts is worth
> the "disaster" that could happen if you miss one of those holes that was
> supposed to move. This is almost as helpfull as the good old autocrap
> days of manually editing a dimension rather than moving the geometry to
> where it is supposed to be and then giving that file to the CNC
> programmer to use for machining.

If you are working on projects that are similar to previous project,
then parametrics can be useful.  But, for the very first design and
there is no idea about what the parts are going to look like, how many
parts are going to needed, or how they will relate to each other then
I have always found references for this stage of a desing to be very
unhelpful.  As far as the issue of managing holes that align this is
why SW developed Smart Fasteners.  I find that it is best to put in
most of the fasteners when most of the design looks pretty good.
Also, some of the folks that went to SW World have described a new
tool in SW2008 that goes through the model to check if all the holes
are aligned properly between parts.... it will be interesting to see
this tool when it arrives.

billyb, I hope that you find this explanation helpful.

Edt