Hi,
I am currently having a lot of difficulty trying to constrain an assembly.
The scenario is this:
I have a sleeve which I am trying to put on a shaft.The hole is quite large in the sleeve. On the side of the sleeve (at 90 degrees to the big hole, is a smaller hole which which goes all the way thorough the sleeve. This hole takes an L shaped handle in order to turn the shaft once it is all assembled (like the handle on a vice). I am trying to insert this L shape into the small hole using INSERT, but the large hole keeps getting selected. I have done the select other button(green button with little left and right arrows) but no luck, it is selecting the big hole as if it dominates the component.
Please tell me:
I am really open to suggestions as this is the most difficult part for me in Inventor.
Thanks,
David.
As Jeff says, it will be easier to help if we actually have the parts, or at least some screen shots. But it sounds as if you are trying to constrain a pin into a hole that is radial through a cylinder, correct?
The insert constraint requires a flat surface and a hole normal to that surface, so you can't use that in this case. Use a mate constraint between the pin axis and the hole axis, then some others (angle, tangent?) to further constrain the pin.
The small hole probably isn't eligable for an Insert constraint if is cut through the bigger pipe. The insert constraint needs a round (flat) feature to work.
You may need to add some workplanes to use as constraining surfaces.
Paul
David, It is not possible to constrain the items you describe using the Insert command, there is no flat surface or plane to constrain to!
Instead, you can use the mate constraint to mate the axis of the shaft to the axis of the hole, then you can possibly use a tangent or another mate constraint to loacte the shaft in the hole, assuming you have suitable geometry to do that, or you could use an offset mate to constrain the origin planes.
Another way is to draw a sketch with a point or intersecting line drawn at the point you wish to constrain and use that sketch to constrain to. You can turn off the visibility of the sketch afterwards.
The possiblities are endless and it will mostly depend on the actual geometry you have to work with as to how you constrain the parts together.
I put together a demo assembly for you, but then realised, you have 2010 and I only have 2012 or 2013, so you wouldn't be able to open it.
If you would like, I can do a video that shows a few different ways of doing it.
@Anonymous wrote:
I actually did an introductory course in inventor, and this was the hardest part I think for most people, including the instructor at times. I had a play around with solid works and found that it constrained a lot easier, .... sometimes you can pull your hair out trying to figure out which it is, I am sure the programme can make a guess as to what it is or a suggestion and speedup things up (it seems to be super clever).
You need to find a different instructor. Constraints in Inventor are completely logical.
I have not found any significant difference between Inventor and SolidWorks (I teach both).
The program as absolutely zero cleverness. It is a software program. Neither the software or the computer has thinking ability.
Once you understand constraints they should be rather obvious.
Inventor is a professinal program and deserves (demands?) a professional level of preparation.
Attach your assembly here if you want instruction.
David, while it would be nice to have some of the icons be a little larger and more descriptive, you have to remember that this software is aimed at professionals. That is, people who have degrees or at least a lot of experience in the work that they do, and for them, the enhanced icons etc... are simply not needed. And that could be the case for you too, soon we hope ... lol
I agree that Inventor, like any professional software, can be difficult to learn, but that in itself is the challenge don't you think?
Imagine what you can achieve if you have a first class knowledge of Inventor.
It's good that at least you have sought some professional help in learning Inventor, but if the Instructor is having difficulty, then as JD said, find another Instructor, because that one is seriously lacking knowledge and that is something that you NEED!!.
I will put together a quick video that shows a couple of ways of constraining for you. I'll post the link when it's done, in an hour or two.
Hi JDM,
Thanks for your comments, I appreciate your help. I managed to constrain all the parts except for the transitional contraint on the pawl and ratchet in this particular assembly. I am getting the warning that i need to delete some other constraint before i do the transitional contraint. Attached is the file, excuse the colours i was experimenting.
Hi Andy,
Thanks for your encouragement and for the help from JDM. Yea I look forward to the day i am natural with Inventor.
Thanks. Look forward to your video.
David.
David, I hope my video helps, I have only shown two different ways to constrain, but I hope you get something from it.
The problem with your pawl and ratchet maybe a measurement issue. The distances between the two parts may be a little off. Use the measurement tool to help sort that out, or use a sketch or planes to constrain to instead of the faces. There's a tip in the video to handle that I hope ... lol
If you have any questions though, just holler.
The video is at;
Well, we have already run into a serious ommision from your class.
It should have been drilled into your head that an assembly file without part files is useless.
An iam file is simply a list of hyperlinks to the ipt part files and a record of assembly constraints.
You will have to post all of the ipt files here as well as the iam file.
Hi,
Thanks for the video you did it was a help. I wasn't aware that I could be flexible in constraining parts like that - I have a lot to learn. I like to have that freedom to be creative with it, but I worry that I would get myself into corner and not be able to make that final constraint.
I also need to clear up what the purpose of a contraint is. Is it simply to show how these parts can be 'glued' together or does it carry a greater weight as being the foundation for for any furture simulation and testing (for example to see the stressors on a piston engine). The reason I find this important is because if I constrain in which ever way I want and still end up with a constrain, would I have done it right to satisfy the more complex Inventor tests and simulations? Would some constrain pathways skew advanced tests and simulations?
Thanks again,
David.
I wouldn't think so, most of the simulation and testing in Inventor seems to lock everything in place and you have to add special case contraints that move or otherwise simulate the conditions you are testing.
Generally speaking, if things are constrained the way you want them to be in the assembly, they will be fine elsewhere.
If you left click on a part, and you cant move it around in any other way than you intend, then it is sufficently constrained. You don't have to go crazy with the superglue .... lol
I often model engines and as you know there are a lot of moving parts in an engine. I can constrain things in such a way that everything works when I spin the crankshaft. The only problem I have is the valve springs, they can't be simulated in the assembly environment, but everything else works, including cam, valves, etc...
Thanks for you help and clearing that up. Hope to chat again soon. JDM is helping me out too with that practice project - I am waiting for his reply.
Regards,
David.
@Anonymous wrote:Hi,
....or does it carry a greater weight as being the foundation for for any furture simulation and testing (for example to see the stressors on a piston engine).
David.
Yes, how you do your assembly constraints is important if you ever get into Dynamic Simulation (an advanced topic quite a ways down the road up a very steep hill).
There are two ways you can do simulation joints, automatically convert assembly constraints to DS joints, ignor the assembly constraints and manually define the DS Joints, or semi-automatically chose what constraints get converted to joints (I guess that is three ways).
In any case, as your assemblies get larger or you do get into DS the importance of best practices in constraints increases. Search here for Walt Jaquith, "House of Cards" essay. (that should be a sticky here maybe someone has it book-marked)
I don't see any attachments.
Do you see the attachments here? (I don't)