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
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.
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.
If you have trouble figuring it out - you might attach your assembly here.
You might create iFeatures to optimize the process.
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.
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.
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.
I don't know how it could be any easier than insert to a surface cylinder?
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.
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..
Try this one. Are you on Inventor 2012?
@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.
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.
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
An extruded surface body cylinder in effect creates an axis with less work and more functionality (Insert constraint now available).
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:
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
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.
video on using joints to do this
https://www.youtube.com/watch?v=1bChwD4mlAA&ab_channel=Cadline