Inventor is fun but....

[Anonymous]

our company is still not using it for real projects. Here's why......

(Sorry if this has been covered but I couldn't find it anywhere)

I thought Inventor was pretty useless for top-down design until Drew showed
me the skeletal design process, and that finally opened up a potential of
use for us, so I feel we have to stick with skeletal design process for our
type of work.

We design machinery that is different each time but, of course, like most,
we reuse a lot of parts or sun-assemblies, for example, a plate for a 1-1/4"
pillow block (at the most basic level).

The thing we (or I guess "I") can't figure out is how do we include that
plate for a 1-1/4" pillow block in dozens of different machines without
redrawing it each time. I think this must be a common problem but I haven't
seen a solution.

Okay a few options as I see them.

1. Use iFeatures to store often used sketches. Fine, but sometimes that
re-usable part is more than just one part. Sometimes it's an assembly of
many parts, that you later have to build onto.

2. You could derive your assembly at some point into a part. Then derive
again this only surfaces, make sketches on those surfaces. Then derive parts
from that, then create another assembly, place the original assembly, and
the new parts created from the new master sketches into the new assembly.
Wow. Seems like a lot of work if the part is just a plate. Plus it would
make a mess of BOM like nobody's business.

3. Derive that part into the master sketch. Fine but I can't move that part,
the program just aligns the workplanes and that won't help. Sure would be
cool, if I had constraints in parts.

4. Create an assembly. Place the master sketch, then place the standard
parts. Now what? I can't derive this assembly to create a new part because
the sketches dissappear when you derive the assembly.

5. iMaster technique (credit this newsgroup) : Good in some applications,
but "I" don't know where the parts are going to go until I create the
sketch, so I can't just constrain the parts to the workplanes because I have
no idea relative to the workplanes.

6. Redraw a quick represention of the already created parts (from third
parties like cbliss.com or parts we had previously created), so that the
skeletal approach still updates properly. This seems to be the only workable
approach but too time-consuming to make it worth it. (why should I have to
redraw something I've already drawn a dozen times when the drawings are
already in Inventor?)


I must be missing something obvious because everyone seems to use Inventor
on a daily basis for real work, but for us without the ability to make a
skeletal master with parts that I can reference with other sketches that I
can then derive into other parts, we can't use Inventor,.......... yet.

Sign....back to AutoCAD

thanks all.....

enric ribas

[Anonymous]

My suggestion would be put the part in a library and then refer to it as
needed. You could constraint the part to a feature or sketch in any of your
skeleton assemblies. That way it would move with any changes to the master.

--
Sean Dotson, PE
http://www.sdotson.com
Check the Inventor FAQ for most common questions
www.sdotson.com/faq.html
----------------------------------------------------------------------------
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"enric ribas" wrote in message
news:C41F53B26F13A571196B43F63AF4C9F2@in.WebX.maYIadrTaRb...
> our company is still not using it for real projects. Here's why......
>

[Anonymous]

Not sure if I understand but I can constrain the part to any assembly that
can include my master sketch, but I can't include parts IN the master sketch
and therefore can't reference any geometry of the parts.

For example, if I have a frame that I have a master sketch with the top
view, and a side view. From that master sketch, I can create the entire
frame. But if I have a set of pillow blocks (or whatever) that I need to
reference in order to make say a shaft 1/2" longer than the pillow blocks, I
need to either draw the pillow block in my master sketch and then reference
those lines in making the sketches for the shaft or ???

Doesn't seem like a big deal in this example, sure, just spend two minutes
and draw the damn pillow block, you lazy *^^%(&^, but in other cases, it's
much more complicated, besides I don't want to have to redraw the pillow
block when Mr.Bliss has already done it for me. (BTW... thanks)

thanks for the response. Maybe I didn't quite get it, though.

[Anonymous]

I know you said you don't know where things go until you start sketching, but can't you
just put them in a assembly, derive that assembly into the file that is to be the master.
Then as you know better where they belong you can adjust their location in the assembly?
Basically you aren't going to build off of faces on parts until you have a pretty good
idea where they belong?


--
Kent
Member of the Autodesk Discussion Forum Moderator Program


"enric ribas" wrote in message
news:0D1A0F7AFD2E68D35D4A54F00A1A39B8@in.WebX.maYIadrTaRb...

[Anonymous]

enric

What do you really expect? IV to automatically know what size of pillow block
that you intend to use in your design and therefore somehow know also what size
based on this your design intent to place a mounting plate correctly to mount
this part. You have to - as current methods dictate no matter what software you
wish to use, to provide the software the necessary information so it can do its
job.

Create library's of std parts to place in your assy - then in your skeleton
represent them with simple stick geometry. Yes you will have to refer to the
catalogue to manually size the sketche(s) to the purchased item. In the case
where you have a mount PL to match the pillow block- chuck in another sketch and
a couple of work planes and you are ready to rock and roll with the plate. Then
you do not have to fully define the purchased part in the skeleton.

The dilemma you are describing is one where there are manufactured items and
purchased items mixed together within a skeleton. You need the purchased item
geometry in there (and you may very well later select a different size making
the time spent valuable for those updates) so the other parts are correctly
placed relative to them making the relationships intact.

That's life.

[Anonymous]

Easy for some folks to forget just how much harder it was to do this stuff
back in the 2D AutoCAD days I guess. Personally, I'm grateful for where we
are now and no matter what I would like to be able to do, doing anything in
Inventor is a pleasure in comparison.
~Larry

"enric ribas" wrote in message
news:0D1A0F7AFD2E68D35D4A54F00A1A39B8@in.WebX.maYIadrTaRb...
> Not sure if I understand but I can constrain the part to any assembly that
> can include my master sketch, but I can't include parts IN the master
sketch
> and therefore can't reference any geometry of the parts.
>
> For example, if I have a frame that I have a master sketch with the top
> view, and a side view. From that master sketch, I can create the entire
> frame. But if I have a set of pillow blocks (or whatever) that I need to
> reference in order to make say a shaft 1/2" longer than the pillow blocks,
I
> need to either draw the pillow block in my master sketch and then
reference
> those lines in making the sketches for the shaft or ???
>
> Doesn't seem like a big deal in this example, sure, just spend two minutes
> and draw the damn pillow block, you lazy *^^%(&^, but in other cases, it's
> much more complicated, besides I don't want to have to redraw the pillow
> block when Mr.Bliss has already done it for me. (BTW... thanks)
>
> thanks for the response. Maybe I didn't quite get it, though.
>
>

[Anonymous]

I have done some pipe carts. The corner pieces, t joints etc are bought and
the pipe is cut to length. I use the adaptive or an excell spread sheet to
size things. If I know that I want a certain centre to centre then that is
stable and any subsequent spacing on the pipe is based off of the origin
planes in the centre of the one pipe. Some lengths are the driving force
and others are adaptive. It works on a medium sized assembly alright.

Kathy Johnson

[Anonymous]

> What do you really expect? IV to automatically know what size of pillow
block
> that you intend to use in your design and therefore somehow know also what
size
> based on this your design intent to place a mounting plate correctly to
mount
> this part. You have to - as current methods dictate no matter what
software you
> wish to use, to provide the software the necessary information so it can
do its
> job.

I don't think that's what I was asking for, but that's a good idea. Sure
would be nice if IV could tell me what size pillow block to use, sort of
like a built-in machinery's handbook.


> Create library's of std parts to place in your assy - then in your
skeleton
> represent them with simple stick geometry. Yes you will have to refer to
the
> catalogue to manually size the sketche(s) to the purchased item. In the
case
> where you have a mount PL to match the pillow block- chuck in another
sketch and
> a couple of work planes and you are ready to rock and roll with the plate.
Then
> you do not have to fully define the purchased part in the skeleton.

Basically, that's what we're doing. I gave an example with a pillow block,
but sometimes it's an entire sub-assembly but used in a different way. So,
yes, we can represent that sub with "simple stick geometry" but it's quite
time-consuming, prone to errors, and doesn't update if I change the sub. It
also seems a bit silly to have to do since the parts are already drawn and
correctly constrained.

>
> The dilemma you are describing is one where there are manufactured items
and
> purchased items mixed together within a skeleton.

Exactly.

> You need the purchased item
> geometry in there (and you may very well later select a different size
making
> the time spent valuable for those updates) so the other parts are
correctly
> placed relative to them making the relationships intact.
>
> That's life.


If by "that's life" you mean too bad for me, then why bother replying?
Otherwise, I don't really get the comment.

thank you for your reply.

[Anonymous]

Unfortunately, not for us. I guess for us it's still a matter of KISS. (Keep
it simple, stupid)

When we get a project and uses a lot of pieces that we already have drawings
for, it's still quicker for us to work in 2D, which is why I'm trying to
find a solution for using parts in skeletal design.

thanks for your reply.

[Anonymous]

Enric

Can you explain more why making a assembly of purchased parts, and then deriving that into
a part file to use for the basis as the skeleton doesn't work?

--
Kent
Member of the Autodesk Discussion Forum Moderator Program


"enric ribas" wrote in message
news:596D9CECE1189D3DCFA46FD68E70FFE2@in.WebX.maYIadrTaRb...

which is why I'm trying to
> find a solution for using parts in skeletal design.
>
> thanks for your reply.
>
>
>

[Anonymous]

If I understand your comments, you mean to follow the iMaster technique, and
have a master assembly from which the master sketch is derived and then plop
down all the purchased parts in the assembly. Then as the design of the
master SKETCH evolves move the pieces within the master ASSEMBLY closer to
where they belong. Is that the idea?

This is the path that I was following, but the only way of moving the parts
in the master ASSEMBLY is by constraining to the origin planes. This is a
very difficult way to get parts into the right place, I think.

I guess I would like parts and assemblies to be the same thing (ala
IronCAD): Have the ability to constrain parts in a part file or have the
ability to create sketches in an assembly. Then I could derive either into
new parts. Maybe IV7 ?

For now, the only solution is to keep redrawing simple stick representations
of existing parts or subs in the skeleton.

thanks for your reply.

[Anonymous]

Basically, it does work, following the excellent example that Sean (I think)
gave on his site with the iMaster technique.

I got very excited and thought that I could finally have parts in my
skeleton. Problem is "I" can't (maybe others can) create an assembly with
the parts in it in the right places because I don't know where they will all
go until I've created the master sketch. I could place the master sketch in
the master assembly to contrain them but that creates a circular dependency
since the master sketch is derived from the master assembly.

I can create a master assembly with all the parts, but the only way to
organize them is to contrain them to the origin planes or to themselves, but
I don't know, for example, the distance between PartA and PartB until I've
worked it out in the drawings. If I could sketch within the assembly, I
could figure out their relationships as well, but I can't.

Am I making any sense?

[Anonymous]

I believe the iMaster example you are talking about might have been mine 8^)

Yes you are making sense, and I can tell you the developers are aware of this issue along
with other issues. I know they have been looking at "POSSIBLE" ways to improve this
method, some not far from the things you are suggesting, but I have no idea ""IF"" or when
any changes will come about.

While I agree it is a bit of a pain to constrain blindly to the origin planes, I
personally don't find it that bad. In reality only 1 part needs to be tied to the
origins, and all others can be constrained to that part and others.

--
Kent
Member of the Autodesk Discussion Forum Moderator Program


"enric ribas" wrote in message
news:8D68BDD643AD97EBA068DE593AC0C2A0@in.WebX.maYIadrTaRb...
> Basically, it does work, following the excellent example that Sean (I think)
> gave on his site with the iMaster technique.


> Am I making any sense?
>
>
>

[Anonymous]

Thanks for your repsonses. I am glad to hear AD is looking into this area,
as in my opinion it is a serious problem with IV, and why we didn't continue
with subscription after 5.3 because we are not using it for real projects,
only for fun little things.

Personally, I think you should combine the part and assembly file types into
one "filssembly" file type that could contain sketches, parts, constraints,
or even include other parts. IronCAD program (which made many other problems
last time I used it) used this idea for its file types and worked very well
and elegantly, so I know it is possible.

I will try more examples using the method you describe.

thanks again.

[Anonymous]

The problem with this idea is, you have all information in one file that has to
load. This limits the size of your assembly greatly. Inventor is unique in that
it decentralized files which make 5000 part assemblies a reality.
--
Dave Jacquemotte
Automation Designer

[Anonymous]

That's not really what I'm saying Dave.

I just meant that the part file is the same as an assembly file. It would
have the capabilities to have sketches, parts, constraints, and other parts,
included, placed or derived within it, but you would still divide your work
into the same structure of 5000 different files. A master sketch, an
assembly, subassemblies, parts, etc., but each file would be the same file
type. Instead of *.ipt. and *.asm they would all be *.inv or whatever.

Of course, for a small project you could contain it all within the same
file.

[Anonymous]

enric

If you wish to instance a master sketch into a master (general) assembly - then
you can.
You can then as you wish constrain parts to the master sketch.

If you are finding that you are getting circular references as you attempt to
instance the sketch then your master sketch has been compromised, by you
preventing this action.

Regards
Kent Mathews