Parametric Feature Suppression

Anonymous · ‎11-16-2003

Has anyone else ever tried to do this? For example, have an extruded
feature exist if parameter Show_Feature is 1, but not if it's 0? And I'm
not talking about iParts - just standard parts.

I've got a little trick to make this work, but if this is already common
knowledge, I'm not going to create an example and explain it. Let me
know.

Brian R.
Iwaskewycz
Senior Mechanical Engineer
PA Transformer
Technology, Inc.

Anonymous · ‎11-16-2003

Other than using VBA I don't know of a
way...

--
Sean Dotson, PE

href="http://www.sdotson.com">http://www.sdotson.com
Check the Inventor
FAQ for most common questions

href="http://www.sdotson.com/faq.html">www.sdotson.com/faq.html
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Anonymous · ‎11-16-2003

Aha... perhaps I should create an example and post it to IVCF?

NO VBA IS NECESSARY.

Anonymous · ‎11-16-2003

You've got my attention...

Anonymous · ‎11-16-2003

But I'll bet that Excel is required, as that is the
only way I know

of where you can put a conditional expression in
the parameter

table. Do you set the extrusion distance to zero in
this case?

Or you MIGHT be able to just multiply the extrusion
value by

Show_Feature, as anything times zero
should also be zero,

though I don't know how Inventor would handle
that.

Bob

Anonymous · ‎11-16-2003

I also know two tricks to "supress" features, so I
am curious what you have in mind...

Anonymous · ‎11-16-2003

See post in IVCF... change parameter "Show_Relief" from 1 to 0 to suppress
the relief feature...

Again, NO VBA and NO EXCEL.

With all the talent out there in this NG, I find it really hard to believe
that I'm the first to come up with this...

Anonymous · ‎11-16-2003

Inventor will not allow you to extrude/revolve a feature by a zero
distance/angle.

Anonymous · ‎11-16-2003

I do not see your post yet, but the solution I
mentioned whereby you multiply the extrusion

(or other feature distance) by either 1 or zero
does not require excel, although maybe I did

not stress that.

Also, as necessity is the mother of invention (or
was that laziness), no one thought of

it because they most likely had no need for
something like that. I typically just suppress

any features I don't want.

Bob

Anonymous · ‎11-16-2003

Hi Brian,

I have taken a look at your example, and for me
that's a known trick, but I am sure this new for quite some people
here

(You should zip your file and post to IVCF, now it
resides unzipped in Customization)

I do have one comment: never, never let a dim
become 0 with the possibility to be enlarged later on. That's a no-no in
Inventor. I know you "solved" this by having a temporarely block on both sides,
but you should avoid this in all cases.

Never-the-less it shows that feature "supression"
is possible without VB.

Cheers,

Teun

Anonymous · ‎11-16-2003

I would have zipped it, but believe it or not, I do not have any sort of
compression software on this machine until the almighty IT department installs
it for me. I'm REAL close to hacking my box to get admin rights on
it...

With the example I posted, I realized (after I posted it, mind you) that I
could have done it with out zero dimensions by dimensioning it from the side
instead of from the center. That would have eliminated the need for the
other "temporary block" that is there just in case the sketch solver puts the
relief on the other side. You never know which way the solver will go in
that case, so in that respect I would agree with you that it's a no-no unless
you take precautions...

Anonymous · ‎11-16-2003

So you used the same concept to place the extrusion
somewhere outside the

part instead. What is the advantage of this over
just suppressing the features

in question? First it seems much harder to setup
and "get it right" as opposed

to just suppressing the features in the first
place. Plus there might be disadvantages

down the road, should Inventor decide to choke on
features outside the part,

as it has been prone to complaining about features
that do not change the number

of faces, etc. in the past.

Bob

Anonymous · ‎11-16-2003

The advantage over just manually suppressing the features is its
ease-of-use and its elegance. I'm currently working toward cataloging and
automating many of the common parts that we create here. The less the
drafting/design department has to think about how to use something that
I've pre-configured for them, the higher the probability is that it will be
right. I "discovered" this technique while creating our transformer
cores. Single-phase transformer cores have only two legs; three-phase
cores require three legs. So if the parameter "Num_Legs" is 3, the middle
leg of the core is shown; if it's 2, it's not there. No one that uses it
has to think which feature(s) to supress.

There is no danger of having a feature not change the number of faces and
choke. There is always some material there for the cut feature to
remove.

Anonymous · ‎11-17-2003

>I find it
really hard to believe that I'm the first to come up with
this...

Sorry to burst your bubble but you weren't the
first...

The main point is that It's not really
suppressed. This can potentially screw up some FEA and CAM software
packages.

But if all you need is a representation then this
is a great trick...

--
Sean Dotson, PE

href="http://www.sdotson.com">http://www.sdotson.com
Check the Inventor
FAQ for most common questions

href="http://www.sdotson.com/faq.html">www.sdotson.com/faq.html
-----------------------------------------------------------------------

Anonymous · ‎11-17-2003

No bubbles were burst. I knew I couldn't have been the first to come
up with this technique.

Parametric Feature Suppression

Parametric Feature Suppression

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