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constraining a hole to a slot

17 REPLIES 17
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Message 1 of 18
folkman1
9937 Views, 17 Replies

constraining a hole to a slot

Good morning,

Is there a way to do this?  2 parts, 1 has a hole in it and the other has a slot.  I want to constrain the center of the hole to the center of the slot.  How do I do this?

Thanks

17 REPLIES 17
Message 2 of 18
Ray_Feiler
in reply to: folkman1

This is something Mechanical Desktop could do but as far as I know in Inventor you need to create a axis or work plan in the part with the slot that is in the center of it.


Product Design & Manufacturing Collection 2024
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Message 3 of 18
KF090
in reply to: Ray_Feiler

The way I typically do this is to constrain the center axis of the Hole to one of the edges (face) of the Slot and then offset set it the distance to the center of the Slot.  Then I constrain the center axis of the Hole to the center axis of one of the Slot radii and then offset it to the center of the Slot.

 

This is the quickest and simplest way I've found thus far that does not require the use of work planes, axii, etc.

Message 4 of 18
JDMather
in reply to: folkman1

If you have trouble figuring it out - you might attach your assembly here.

You might create iFeatures to optimize the process.


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EESignature

Message 5 of 18
mcgyvr
in reply to: JDMather

When I do a slot (obround) I add a cylindrical surface extrusion in the center of the slot to use to insert constraint bolts into it.



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Message 6 of 18
Ray_Feiler
in reply to: folkman1

As far as my approach goes inside Inventor, I constrain the parts together using their respective work planes where possible and then use the face of the slotted part and the axis of the hole part for the hardware. See attached IV2012 assembly.


Product Design & Manufacturing Collection 2024
Sometimes you just need a good old reboot.
Message 7 of 18
folkman1
in reply to: folkman1

Thanks for the tips.  I was hoping there was an easier (better) way to do this.

Kind of surprised that there isn't.

Anyway, thanks again.

Message 8 of 18
JDMather
in reply to: folkman1

I don't know how it could be any easier than insert to a surface cylinder?


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Message 9 of 18
folkman1
in reply to: folkman1

I can't open the sample assembly that was posted.  I get error messages.  I'm not sure what a "surface cylinder" is.  This is probably a short coming on my part.  I didn't mean to insult anybody, I just thought that picking the center of a slot shouldn't require adding other geometry. That's all. Again, thanks.

Message 10 of 18
mcgyvr
in reply to: folkman1

To create a "surface cylinder" simply create a new sketch with just a circle in the center of your slot. Then extrude (but pick the surface output option instead of solid option) (see attached file)

 

Its as simple as it gets now..



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Inventor 2023 - Dell Precision 5570

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Message 11 of 18
Ray_Feiler
in reply to: folkman1

Try this one. Are you on Inventor 2012?


Product Design & Manufacturing Collection 2024
Sometimes you just need a good old reboot.
Message 12 of 18
JDMather
in reply to: mcgyvr


@mcgyvr wrote:

Its as simple as it gets now..


Creating as iFeature (I use as Punch even if not sheet metal) make it as easy to place and size as any Hole feature.


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Message 13 of 18
Doug_DuPont
in reply to: folkman1

What I do is on my slot sketch I have a center point. When I constrain I turn on the slot sketch and constrain the hole to the center point in the sketch.

Douglas DuPont
Inventor 2016 Pro, Vault 2016 Pro
Quadro M4000
Windows 10 64 Bit
Message 14 of 18
markc-uk
in reply to: Doug_DuPont

It's good practice to put a workaxis at the centre of any slot. Try this workflow that's detailed in the animated .gif attached for a tidy way of placing the axis.

edit - you need to save it then right click on it and open with Internet Explorer

Message 15 of 18
JDMather
in reply to: markc-uk

An extruded surface body cylinder in effect creates an axis with less work and more functionality (Insert constraint now available).


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Message 16 of 18
Hunteil
in reply to: folkman1

I'm seeing a lot of ways / methods to constrain to a slot. I still have 2 ways that aren't listed yet lol. I think Autodesk should have a methods guide for this. Showing all the methods and giving the cleanest method first. B/c some of these methods can cause people more work over others. Example: Like turning on a sketch of a part to constrain to a center point will associate / make the parts adaptive to each other causing Vaulting issues later. Not knocking that commenters way of doing it. It's just good to plan ahead.

 

My other ways:

  1. Constrain the screw / bolt equally halfway between both ends of the slot radius ends. (requires two constraints and knowledge of the spacing between them. Works best if the number is a whole number. i.e. slot is 1" long from center of radius', constrain screw / bolt axis to radius axis =1"/2...then repeat for opposite end of slot. If it's not a whole or even number you may get errors. These 2 constraints is all you need at this point.
  2. Transitional constraint and Joint constraint Type Slider... It's far more complex than I like doing... But works great for parts that move around.
  3. I believe Bolted connection can too... if your company has it setup... We don't so I forget.

I wish I knew how to use ifeatures for the insertion point constraints.... It doesn't work for me.

Model States is not a replacement for iParts / iAssemblies. It does not have all the same features yet and does not communicate well with our large currently in use libraries. 😞 https://forums.autodesk.com/t5/inventor-ideas/model-state-support-tabulated-parts-list/idc-p/11360616

Message 17 of 18
james.willo
in reply to: folkman1

Joint joint joint joint joint. Every time. Joint.

The OP is from 2012 when I don't think joints existed. 

But Joints, no question.

 

 

 

Joint.

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