I am quite new and learning my way through Autodesk Inventor. As of now I am stuck with an issue. I am trying to place the following part
inside this shelled box.
I had made the U bar (the first part) as adaptive and the sketch for the sweep profile is also made adaptive.
I am trying to place this U bar inside the shelled box's inner bottom area and make the U bar to change its size with the bigger box.
I learnt about adaptive feature and experimented with a cube as shown in http://www.youtube.com/watch?v=uH4RsonLY5o.
However I am unable to add constraint to make it happen. I am attaching the IPT files of the two parts and one IAM file. The 'sick' alignment is what is troubling me. I wonder why this works in the video and not in my part.
Could some please shed some light?
Solved! Go to Solution.
I usually use derive instead of adaptivity - ignorance more than anything else I suppose :-)
I found the tuts here, including adaptivity very successful though. http://www.mcadforums.com/forums/viewforum.php?f=4
In the future it is always a best practice to tell readers here what version of inventor you are using. It appears these are version 2014. A lot of us here are still on 2013.
Since I also had 2014 on my computer for evaluation I was able to open them. What exactly are you trying the get to change on the bar, the diameter or the length of the legs?
My apologies for missing Inventor's version. Yes, I am using Inventor 2014. In future if I need to attach any Inventor files, I will save as to old version and upload mentioning the version.
My aim is to model reinforcement bars. I am trying out various options of Inventor to do so, that's my overall intention. With regard to this question, When the shelled box's size changes, I want the U bar's leg lengths to change and to fill in the shell of the box.
You cannot save backwards to an earlier version in Inventor. Just let us know what version you have, someone will help you.
I noticed first of that your sketches and sweep are NOT adaptive. I deleted the sweep, and profile sketch. Then made sketch10 adaptive by right clicking the sketch and selecting adaptive from the menu. I did the same with the profile work plane. Then remade the profile sketch and made it adaptive. When I remade the sweep it was automatically set as adaptive due to the sketches adaptivity.
In your assembly, you must also right click the part and set to adaptive there. Now,... all of that said and done.... I still cannot get it to work. I admit, I have never attempted adaptivity on a sweep, and there may be something about the geometry that is preventing it. I will continue to play with it for a while (I do have a tiny bit of work to do today... but not much). But if I were you, I might start looking into other ways to do this.
Frame Generator is one possibilty, but it is a bit more advanced. I would start with some tutorials before diving in.
If I get anywhere I will post back, meanwhile anyone else who has done more with adaptivity than I is welcome to jump in here.
It seems to me that adaptivity does not need to play a role here.
While I do not have 2014 yet and still on 2012 (so I cannot open your parts) what I am thinking is if you turn off the adaptivity and use this mate tool
to mate the tube to the box you will have your base parts mated together. But, actually before you mate them together to create your assembly, I would first create factory files of each part so they have all of the sizes you need. Then once the factory files are created, create your assembly of them and then ultimately make the assembly a factory (iassembly) as well to interchange all of the sizes.
Hope this helps.
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I'm not sure why you want to do it like this, but take a look at this method.
I noticed that none of your sketches in the u-bar were constrained. This is why it isn't working. Not only does your part have to be set to adaptive, as Chris mentioned, but your sweep path must be constrained to the edges of the Slab part. To do this, you have to project the slab edges into your sweep path sketch, then constrain your sweep path to those projected edges.
Take a look at Ray's assembly. He has done exactly this.
The sketch constraints are the thing that tells the path how to adapt to the other part, not the assembly constraints (at least with this example).
I'm used to doint this with straight parts made form extrusions. I leave all dimensions and constraints off the sketch and set to adaptive in both the part, and then the part in the assembly. usually works just fine, but this is a sweep... I figured the rules were prolly different.
Yes, you're right. I tried it with a simple extrusion, and it behaved just like you describe. I guess sweeps are different, for some reason. In fact, when I tried to follow the same steps with the sweep, I noticed that there is no option to make the sweep feature adaptive:
I was able to make the path sketch adaptive by setting it BEFORE I created the sweep feature (can't be done after the sweep is created), but this wasn't enough to make it work.
Instead, I was able to get it to work by creating a work plane, making it adaptive, and constraining the path sketch to the work plane. Then, in the assembly, I constrained the work plane to the slab part. This worked. See the attached assembly (Inventor 2014).
As an aside, the only time I ever use adaptivity (and only occasionally) is when creating flexible tubes between fittings that can change position (when I don't want the overhead of using the Tube & Pipe module). But these usually involve 3D sketches for the sweep path, and I have found that there are special techiques required to get the adaptivity to work with 3D sketches.
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