Constraining assembly components.

[Squawk]

My intention is to make a foam inlay for a component.

The foam inlay however is not a square but has both tapered and little round sides.

I can make a "mate - flush" constraint and get the component to align the correct place in height.

But I can't find any way to constraint the closest proximity of the object to 1 mm from the sides.

Is there any way I can accurately set the position of the component from the sides, preferably constrained?

Please see attached file.

Thank you for any help in advance!

[mcgyvr]

Don't forget you can constrain to origin/work planes (user created planes)..hint hint.. 🙂

[swalton]

One choice is:

Tangent with a 1mm offset between the cylindrical surface of the part and the planer surface of the case.

Add an angular constraint to keep the part from rotating.

If you were smart about symmetry and your origin geometry when you created your ipts, you might be able to use the origin planes.  That will depend on what you want driving the assembly. 

[Squawk]

Thank you McGyvr, I have to look up how to do that..

[Squawk]

Thank you for your reply Swalton.

I'm affraid I wasn't smart when I created these parts and have not based it around the centre point.. 😞

I tried the tangent constraint with the 1mm like you said, but I kept getting weird results.

The component went through the side, instead 1mm away from it..

And it also rotated.

Problem is, since there is no horizontal reference (the sides are a bit round) I can't get the angle to restraint to anything..

[swalton]

Tangent may have an issue with the tapered case walls. I read your question too quick and did not see that part.  Tangent has two solutions, basically one is inside the circle and the other is outside.  You might try playing with the solution options in the constraint window.

A mate constraints will work between a planer surface and an edges/axis/vertex.  This might get you where you need without creating work geometry. 

If you attach your ipt files, I may be able to take a look and see a solution.  The iam file that you attached is basically a list of the locations of the part files and the constraints between them.  (Also, I am on IV 2014. if you are using IV 2015, I can't open your files anyway.)

The lession is:

Plan your part modeling by how you need to use the parts later in your assemblies and in the real world. 

Don't forget to consider how you might want to modify the part for some future use that you don't know about yet...

It takes a bit of practice to get there.

[JDMather]

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@Squawk wrote:

Please see attached file.

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An assembly file (*.iam) is only a list of hyperlinks to the part files (*.ipt) and a record of assembly constraints (and a bit more).

You must include the part files.

[mcgyvr]

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@Squawk wrote:

Thank you for your reply Swalton.

I'm affraid I wasn't smart when I created these parts and have not based it around the centre point.. 😞

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So..now you know better and can simple edit the parts first sketch and fix that problem.. 

[johnsonshiue]

Hi! There should be several ways to constrain the components desirably. Mate, unlike Flush, is a fairly versatile constraint allowing combinations of vertex (sketch point, edge (sketch line), and face to be constrained together.

Thanks!

[Squawk]

Yep, sorry, .iam and .ipt files attached..

Indeed I get weird results trying to constraint the component in ways I know. Probably due to the tapered sides..

I'm on Inventor 2012, so you should be able to open them.

Thank you for offering to look at it!

[Squawk]

I don't understand.. I have only 4 options to constrain components: Mate, Angle, Tangent, Insert.

But either way, I cannot find any points, axis, surfaces or other things to constraint to in such way, that the component doesn't stick out the foam block in the tapered place where it is closest to that component.

All google and youtube searches only show constraining using one of the 4 above mentioned.

Obviously I need another way. And folks here say there is, but I can't find it..

[JDMather]

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@Squawk wrote:

My intention is to make a foam inlay for a component.

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I thinking was Derived Component would be easiest technique.

[JDMather]

Open the Case file.

Manage>Derive Component and select the Phantom 2.ipt file.

Select Move Body and enter the following dimensions to center

Combine with Cut option to create the cavity.

Now you can assemble the two parts in an assembly file.

[Squawk]

Thank you for your help JD!

Your example saved my day.. 😉

But, my aim is to have it 1mm from the closest point to the tapered side of the foam block, on the left top side.

(There is other stuff that needs to go in there.)

How can I let the program decide that?

I could get it by entering values untill none of the pod poked through the tapered wall, and then add 1 mm for some margin.

But I thought the idea of Inventor was to let these things be calculated/constrained.

I felt like the unsymmetric drawing approach noob earlier when doing this on trial and error value entering..

Just 1 question left, you said: "Now you can assemble the two parts in an assembly file.", but with what I now did was make my case .ipt file with the holes in it for the components. It's not an assembly file anymore, but a .ipt file.

Or did you mean that I can assemble the Phantom in the case with that now have the holes, in an assembly file?

[WHolzwarth]

You could do that easier, by modeling the case symmetrical to at least one original plane. I've "re-invented" 😉 two planes for constraining. Now you can change position of the phantom part easily.

Only modified files are added (2012).

Walter

[JDMather]

I would have modeled all of this using multi-body solids in the orientation I wanted and then pushed out the assembly.

But I don't think you are there yet.

Just keep working.

[Squawk]

Thank you for your reply and sample file Walter!

I made some items in the tree visible to see what they were.

If I understand correctly, you changed the position of the Phantom center point, then made 2 work planes throught that center point of he Phantom component and made 2 work planes on the sides of the case.

But when I change the "Passend" values of the Phantom, the work planes remain the same position, but the Phantom moves in relation to the work plane.

Why did you need the 2 case work planes then?

And how did you manage to create a work plane that didn't follow the tapered shape of the case sides?

[Squawk]

I would have modeled all of this using multi-body solids in the orientation I wanted and then pushed out the assembly.

But I don't think you are there yet.

No, I don't think so either.. 😉

But just to be sure, following your way, I don't end up with a Assembly .iam file, but with a Part .ipt file that has the holes in it from the combine function.

Right?

[JDMather]

The real world ends with an assembly.

I would end with an assembly created from the "pushed out" derived parts.  (Manage tab>Make Components)

I suspect there is a tutorial covering the multi-body solids and Make Components in the Help>Learning Tools>Tutorials.

I know there is a tutorial covering this technique on my website (Vacuum Tutorial).

[Curtis_Waguespack]

Hi Squawk,

I have 2 solutions for you try, in order to help you get these parts constrained how you'd like:

1) Edit each of your parts and use the Move Body tool re-center them on the origin, then you can use the origin planes to create assembly constraints:

http://inventortrenches.blogspot.com/2011/06/change-origin-of-imported-model.html

We do this a lot when we import parts that are off center, but you should be able to use the same trick to re-center your parts.

 OR

2) Since your parts aren't centered about the the origin planes, you can create your own work planes to use to create assembly constraints:

• Start by creating work axes using the cylindical faces.
• Then use those work axes to create a work plane.

(my version of the drone model)

• Repeat for the other side:

• Next create centered work plane by selecting the first two planes. The 2 planes define the new midplane:

• Do the same for the direction, and you should then have more than enough work planes to work with in this part:

• It might help to right click on some of the planes and turn them off, just to reduce the clutter:

Open the foam part and create work planes in the center by selecting midpoints along the edges. 3 points make a plane:

• Same thing for the other direction:

• You'll end up with this:

Now you can mate/flush these planes together in the assembly. If a mate flips the model, then try a flush.

Here's a link with some "how to create work planes" vidoes:

http://help.autodesk.com/view/INVNTOR/2014/ENU/?guid=GUID-80FC6839-D432-4E7E-85C6-0F77E9AEDCC7

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com