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You everybody know, there is a problem at working with bolted connection for slot holes. Bolted connection feature can't recognise slot pockets. As if we show it center of slot, it can't work truelly like on the last image.
I often make slots from a bolted connection hole to allow for adjustments. I would find it handy if this could be done straight in/from the connection. Ofcourse there are issues like if you want a centered slot or an offset slot. And the orientation relative to the part(s). A curved slot would be nice to. Especialy since you have added these 2 slot types to Franklin.
And provide slots to the hole feature as well. Sometimes you want to create an hole into a slot feature.
i-feature isn`t a solution. It only one at the time on each sketch point (so you have to create every slot one by one) and its take too much time to place a i-feature.
(i-have seen on video`s that Solid Edge has it since the latest version)
They definitely need to come up with more complete workflows for slots in general, including constraints/joints that allow for natural movement between them.
For this specific problem, one work-around is to create one or more work points in the part(s) with slots using the "center point of loop of edges" method, and then select that when using the "on point" method for bolted connection.
Not perfect, but I find it MUCH nicer than dealing with the "linear" bolted connection method.
Oh, you don't need to use the "Bolted Connection" tool for constraining the hardware. I just find it to be way faster to use in most cases, if all you're adding is stuff like bolts, nuts, and washers (or other similar CC parts).
You can use the created work points and/or axes to directly constrain stuff to slots. Depending on your needs and circumstances, you can also use the JOINT command to fairly easily assemble hardware to slots.
Your these solutions are great. Many of us try different ways to solve the problems. But why do we make these? Inventor does not have function to make slot holes (this is my another solution idea. You may vote) or bolted connection solution for slot holes.
I do something similar as @chris. The only difference is I leave a solid in the middle of the slot. These are .06 can be smaller. Easy to select. Doesn't affect the laser cut. It won't show in the flat pattern since the center is not connected to the remaining solid. I do a lot of structural connections like this. Makes life easier.
Tip if its a sheet metal part you can place disconnected solids in the model as helpers for constraining and they won't show in the flat pattern. Play with it. I will use this technique on curve parts to help constrain bolts to a curved surface. Say a curved conveyor side with bolt-on/welded parts.
@CStilesCARE - Yep, I use something like this. I have quite a few parts which I have created in a library like conveyor trough sets which have slotted holes. I added a bigger hole to the middle as you have shown.
@jnewon - This is turning the problem on its head - I like it and will try it next time one comes up.
Both however avoid INV from finding a solution by itself - It maybe one of those situations when there could be 2 or more solutions and INV would just flip between each whenever a recalc was performed?
Almost like we need an extra constraint like with the angle constraint setup-a reference face
@lance8 I believe it was @chris who suggested creating a larger hole in the center to use as reference.
My thing was just creating work points and/or axes from sketch points and constraining with them (when invisible) by selecting from the model browser.
This is possibly just personal preference, but I don't like the idea of adding features to a model that modify the resulting output part, because it means it'll be less accurate compared to the real-life version. You could argue this is just being picky, but it can cause (and has caused, for me) issues if someone has to then deal with those alterations later, for example, to correct the cut profile for a CNC machine to use.
I'd rather take the extra 0.5 seconds to locate the part in the browser tree and constrain with work features that won't affect the "output" part model, and have customized my mouse marking menu (right-click + drag in certain direction) to make changing between component & single part select modes easy (see settings snip below).
If interested, my general workflow is below:
ctrl+right-click & select part priority
select part, right-click and select "find in browser" from drop-down menu
expand the node to show desired work features,
repeat 2-4 with other part(s), if needed
Create the constraint(s) by using work features (no need to make them visible - they show temporarily when you mouse over them when selecting for constraint creation)
collapse nodes (if desired) and change back to component priority once done.
