can't drag parts after placing first constraint

[w.hess]

after the first constraint I can't drag the part,

only thing i can do is use the rotate command

[Anonymous]

Any constraint? What constraint are you using and between what types of surfaces? Some constraints can take away more than 1 DOF, so possibly that's what's happening? -- Rui "w.hess" wrote in message news:23776724.1095885970169.JavaMail.jive@jiveforum2.autodesk.com... > after the first constraint I can't drag the part, > > only thing i can do is use the rotate command

[Anonymous]

Do you have any assembly level sketches? "w.hess" wrote in message news:23776724.1095885970169.JavaMail.jive@jiveforum2.autodesk.com... > after the first constraint I can't drag the part, > > only thing i can do is use the rotate command

[w.hess]

I will double check, I don't think so

[w.hess]

any constraint, just a simple mate constraiint

[Anonymous]

Can you reproduce the problem in a new assembly file with a couple of test parts? If so zip and post the iam and ipts.

[w.hess]

These parts were created in the assembly, by the create a new component command. The part can be moved freely ubtil aI place "one" and only one constaint on it I cant move the part anymore. Just with one constraint.

It nearly impossible to work like this.

I

[Anonymous]

Isn't that how it works? When you create a component, you automatically get 2 DOF constrained? I hardly ever (if ever) use that, so I'm not sure. If you create the component, are you projecting any geometry to create the first sketch? Try without projecting any geometry. Seems to work ok with a simple test I ran. -- Rui "w.hess" wrote in message news:19514586.1095946394660.JavaMail.jive@jiveforum2.autodesk.com... > These parts were created in the assembly, by the create a new component command. The part can be moved freely ubtil aI place "one" and only one constaint on it I cant move the part anymore. Just with one constraint. > > It nearly impossible to work like this. > > I

[w.hess]

Rui,

The constraint I am placing only is removing one dof.

The weird thing is when I selected the part to drag, the staus line in the lower left of inventor screen tells me part is "dragging" or "preparing to drag" but the part won't move.

The software trys to execute the command, but won't , this is strangest thing, what am I missing, a setting? please dont tell me I have to reinstall? I rebooted,

I will try a new iam file maybe the one I am using is corrupt?

Suggestions?

[w.hess]

I will try this, thanks for the lead!!!!!!!!!!!

[Anonymous]

I think you need to clear this check box Attachment not added (content type not allowed): "screen1.jpg"

[Anonymous]

When you create a part in the context of an assembly an assumption was made that 9 times out of ten you will probably want the part to be constrained to the face that you used as your sketch plane. So a constraint was created to that face by default. Optionally, you can clear that. Any geometry that you then use from another model will also project across adaptive (by default) meaning that there is a relationship from that geometry to your new part feature - meaning lost degrees of freedom. You can turn that behavior off via the Tools|Application Options|Assembly tab by clearing the checkbox next to: Enable Associative Edge/Loop Geometry Projection During In-Place Modeling

[Anonymous]

Can you grab a corner and rotate? Is it a cylindrical part? What does the Degrees of Freedom show? K Johnson

[w.hess]

not a cylindrical part. i will check dof

thanks

[w.hess]

Hey everybody,

Fixed!

Some how, I had my setting to enable "adaptivity" as I created new components in an assy. file. causing my part to reference other parts geometry.

I had to create a new assy. and re constrain the parts.

Thanks
william

[Anonymous]

Thanks for the notification of resolution and how you fixed it!! "w.hess" wrote in message news:20678721.1096035156928.JavaMail.jive@jiveforum2.autodesk.com... > Hey everybody, > > Fixed! > > Some how, I had my setting to enable "adaptivity" as I created new components in an assy. file. causing my part to reference other parts geometry. > > I had to create a new assy. and re constrain the parts. > > Thanks > william

[will_hebden]

Another reason this can occur is due to a constraint conflict in a different area of the model, fix the constraint conflict and the dragging issue will be resolved.

Kind regards

Will

[Ben.Paterson]

I had this problem too, but found that I had another broken constraint in my assembley,

check your design doctor isn't red and if you have any broken constraints fix suppress or delete them,

not sure if this is what is causing your problem, but thats how i fixed mine

[JDMather]

You have responded to a very old thread.

Hopefully in nearly 9 years - the OP has figured out the problem.