Constraints freezes the part

[Anonymous]

Hello!

This is making me nuts!

When I place ONE constraint between two parts, I cannot place a second constraint. The parts are already frozen.
I cannot drag around the parts. It doesn't matter what type of constraint it is. For example: I place a constraint with two holes together, I should be able to turn one part around this hole. But I can't. When I try to drag it around, there is a symbol like this Ø that normally appears when all possible constraints are set.

Please help me. I have lost almost a day of working because of this. This problem occured yesterday. Before that, I had no problems.

Kind regards
David

[Anonymous]

check the part you want to move isnt grounded...

hold shift+e to show degrees of freedom for the part, has it got any?

sometimes you have to LMB and hold on the part if your assembly is big, give it a few seconds before it will move but as you are getting the circle with a line thru it, this means it cant move

[Anonymous]

Thanks for your reply...



No it's not grounded. There is "no visible unadapted sketches" when I press SHIFT+E.

When I LMB it shows the symbol as you described. But WHY can it not be moved? I have only ONE constraint on it...

[Anonymous]

This is the second similar post in two days. First posted
yesterday by flbonham. Can you provie a zipped example of this problem (assembly
AND affected parts, along with the version and service pack number of Inventor
that you are using. Also, have you updated Windows lately or had automatic
updates on ( not saying this is the issu, just ruling it out)

To post on the Autodesk.Inventor discussion group, the file
must be zipped and under 1.5 MB.

For larger files:

href="http://interlancentral.com">http://interlancentral.com
.
 
Read the instructions on the home page link. No limit on file
size.

WHEN POSTING ASSEMBLY OR IDW/DWG FILES:

Make sure you include all part files along  with the assembly (.iam)
file. When posting IPN/IDW files, be sure to attach all related ipt and iam
files as well.

Please notify in this thread when you have posted the files. Be sure to
note the version of Inventor used.

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[Anonymous]

I'm using Inventor Suite 2009 with SP1 along with Windows XP Professional SP3.

I couldn't get that FTP thing to work, so I uploaded a ZIP here instead:

http://www.sendspace.com/file/92jbfn

[JDMather]

First thing I noticed is that your sketches are not constrained and making any use of symmetry about the origin. I would read this document while someone is finding your problem http://home.pct.edu/~jmather/AU2007/MA105-1L%20Mather.pdf

[JDMather]

I would have done Part S1-1293-30.ipt as a Contoured Flange rather than folding a flat. Your nice even flat dimesions (missing) will not result in nice even folded dimensions.

[JDMather]

Using sketletal modeling techniques and the Frame Generator most of the frame could have been done without assembly constraints.

[JDMather]

I think Inventor should have given you an error earlier. I suspect the problem is with constraints Mate43, Flush35 and Mate104. Let me take a closer look at part S1-1293-13

[JDMather]

I'm not familiar with your actual assembly workflow - but appears there should be some sub-assemblies.

[JDMather]

Mirrored and/or patterned components would have reduced the complexity as well.

[Anonymous]

The first thing I see when I turn on Degrees of Freedom (View
> Degrees of Freedom) is the attached error message... might be a clue.
No time to investigate further.

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[Anonymous]

Which part are you trying to drag?

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[JDMather]

Constraint Flush35 seems to be the problem. I haven't figured out why. I would have placed that or one of the center parts as the first part in the assembly and built symmetrically around the assembly origin planes. I'll leave it to Autodesk or someone else to figure out the exact problem and why it occurred. I would do the parts and assembly much differently - I think you are doing too much work. This could be significantly simplified.

[Anonymous]

S1-1293-30

[Anonymous]

JDMather: Thanks for your tips. I'm not very skilled of Inventor yet.

[Anonymous]

Problem solved. Demote all parts EXCEPT S1-1293-30 into a new
assembly. Reconstrain S1-1293-30 to the same location. See attachment. Info
on Demote and Promote is available in the Help files.

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[Anonymous]

Be sure to groud the new assembly after creation. Your
constraint problem was caused by too many constraints within one assembly,
probably confusing Inventor. The proper procedure in designing anything is to
create sub assemblies on-the-fly within the main assembly file. Each subassembly
basically functions on its own. If you have problems understanding what should
go into each subassembly, make a trip out to the shop to see how the assemblers
build a machine.

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Expert
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HP zv5000  AMD64 2GB - Geforce Go 440, Driver: .8185
XP
Pro SP2, Windows XP Silver Theme

href="http://teknigroup.com">http://teknigroup.com

[Anonymous]

I just ran into a simular problem the other day.
Inserting a hinged "Jaw" into a assemble, had two constraints on the
jaw, the first was a face mate and the second was a mate at the axis hinge
point. The Jaw would not pivot, traced it down to a rib that wasn't fully
constrained. As soon as I placed the third constraint on the rib the Jaw
hinged as it should. 

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style="PADDING-RIGHT: 0px; PADDING-LEFT: 5px; MARGIN-LEFT: 5px; BORDER-LEFT: #000000 2px solid; MARGIN-RIGHT: 0px">

<JDMather> wrote in message
href="news:6062480@discussion.autodesk.com">news:6062480@discussion.autodesk.com...

First
thing I noticed is that your sketches are not constrained and making any use
of symmetry about the origin. I would read this document while someone is
finding your problem
http://home.pct.edu/~jmather/AU2007/MA105-1L%20Mather.pdf

[Anonymous]

Hi,

I forwarded this to development.

Loren Jahraus

Autodesk Inventor Product
Design