What is wrong with this part

[Adam Y.]

Im really confused about this part. Sketch one needs two more dimensions except I have no idea what the sketch actually needs. There might be some lines that Im missing which can be causing the problem but beyond that I have no idea what the missing dimensions can be.

[DonRotolo]

Hard to determine without Inventor loaded...

[zachjo]

I am not sure that you have any problems with this part. I opened it and there were no errors. Looks like a solid square bar with two holes drilled on the two long sides. What is the part supposed to be?

[popo308]

I opened it as well and found nothing wrong with it...

[Bethany Mc.]

Well what are you trying to do with this part. If you are trying to make it fully constrained, all you need to do is add a fixed point, and sketch 1 will be constrained. Other than that it looks fine. If you state what you are trying to do with the part, I might be able to help with greater detail.

[David Guzman]

I opened it up and it looks fine. Do you just want to get rid of the sketch?

If so, all you have to do is go under extrusion 1 and extrusion 2 and right click on the sketches and click on visibility.

More information will help us help you.

[Adam Y.]

Originally Posted by Bethany Mc.

Well what are you trying to do with this part. If you are trying to make it fully constrained, all you need to do is add a fixed point, and sketch 1 will be constrained. Other than that it looks fine. If you state what you are trying to do with the part, I might be able to help with greater detail.

Thanks. I was trying to fully constrain the sketch. Now why did I need to do that for my one part and the two other parts which are essentially the same drawing?

[Bethany Mc.]

Originally Posted by Adam Y.

Thanks. I was trying to fully constrain the sketch. Now why did I need to do that for my one part and the two other parts which are essentially the same drawing?

Well if you want a fully constrained part, you must have a fixed point, or a demesion based off of the orgin. I'm not sure why you didnt need to place a fixed point on the other two parts. I would need to look at them.

[Pat Roche]

I agree with the above posts saying that you are under constrained. Many people, however don't understand why you need to fully constrain your part. The main reason you constrain off the origin is that it allows you to constrain your assemblies easier. Rather than constraining off a side you can constrain off your planes which allow for easier changes (and alot less mental math) later. Also doing this allows easier use of the parameters feature in Inventor. Parameter allow you easily change dimensions of a part and when based off the origin it just gets easier. The easiest way to constrain your part is to go into the 2-D Sketch Panel>Project Geometry then click the two axis you want from the origin tab of the model panel. All thats left is to dimension your part off that.

Hopefully that was helpful,


-Pat

[Adam Y.]

Originally Posted by Pat Roche

I agree with the above posts saying that you are under constrained. Many people, however don't understand why you need to fully constrain your part. The main reason you constrain off the origin is that it allows you to constrain your assemblies easier. Rather than constraining off a side you can constrain off your planes which allow for easier changes (and alot less mental math) later. Also doing this allows easier use of the parameters feature in Inventor. Parameter allow you easily change dimensions of a part and when based off the origin it just gets easier. The easiest way to constrain your part is to go into the 2-D Sketch Panel>Project Geometry then click the two axis you want from the origin tab of the model panel. All thats left is to dimension your part off that.

Hopefully that was helpful,


-Pat

Yes it was. I originally had a hunch that it had something to do with the constraining off the origin because I read it in a tutorial. The only problem was the tutorial mentioned it in passing.

Here is how I would have done the part. Notice that the Feature tree is much more simple.
And note: The holes you used for a 4-40 UNC screw are too big - the screw will fall into the hole as there will be no threads. The screw diameter is .112 and your hole diameter is .112, thus no thread engagement. The correct tap drill size for a 4-40 UNC is a #43 drill (.084"). If you use the Hole tool to create your tapped holes Inventor will automatically assign the correct tap drill size.

Thanks that is much simpler.

[JD Mather]

Originally Posted by Adam Y.

Sketch one needs two more dimensions except I have no idea what the sketch actually needs.

Sketch1 is not constrained to the origin.
Read this document http://home.pct.edu/~jmather/AU2007/...7;20Mather.pdf
especially Tips 8-22
here is your fixed part. Later when I get a chance I will post another part the way I would have done it.

I do not grade student work that Sketch1 is not fully constrained.

[JD Mather]

Originally Posted by JD Mather

Later when I get a chance I will post another part the way I would have done it.

Here is how I would have done the part. Notice that the Feature tree is much more simple.
And note: The holes you used for a 4-40 UNC screw are too big - the screw will fall into the hole as there will be no threads. The screw diameter is .112 and your hole diameter is .112, thus no thread engagement. The correct tap drill size for a 4-40 UNC is a #43 drill (.084"). If you use the Hole tool to create your tapped holes Inventor will automatically assign the correct tap drill size.