I used an AutoCAD technique to solve this

[rickduley]

I am working on a textbook exercise in Inventor 2015.

The given drawing is quite hard to follow.  Actually, the resolution in the graphic above doesn't look too bad, but I have attached a PDF which might be more legible.  For those with a decent library or access to one, the book is 

Giesecke F.E., Mitchell A., Spencer H.C., Hill I.L., Dygdon J.T., & Novak J.E. (2014). Technical Drawing. Upper Saddle River (NJ) USA: Prentice Hall

and the exercise is 6.103 Lever Bracket on page 210.

Also attached is an IPT file which is the best I have been able to achieve so far with thise exercise.  I have had to change some of the dimensions to get an acceptable product, but there are still a few unresolved mysteries.

The first of these mysteries is creating the base plate.  The dimensions are given relative to the centres of holes which cause me a bit of a headache.  I resolved the problem by resorting to an AutoCAD technique which is laying out a dimensioned grid (Sketch 1) then outlining according to that (Sketch 2).

The question here is, "Is there an easier, more efficient, Inventor Style way of creating the part?"

Thanks

[blair]

Not really sure why you did Sketch1, it's not constrained (grab and drag the RH Upper corner) and really a waste of time. Make use of the Origins, Sketch2 should be your primary sketch and a number of users would use the Boss hole to be located at the Origin Point. Feature6 could be a simple cut out of the back-side.

I don't have my reading glasses at my desk at home, I did a quick model of the base. I didn't constrain the Upper LH straight edge as the PDF is pretty blurry. It should give you and idea, I also Shared the base Sketch1 to use for other features.

[nmunro]

Here is an example of how you might approach it. Try to lay out the interface features (typically hole and bore locations) as early as possible. A few dimensions did not make sense and others in the pdf were hard to decode so it a bit of a guesstimate. The resulting IV model is much much easier to change than a 3D AutoCAD solid (created using non parametric solids).

Model is IV2014 format.

[rickduley]

Hi Blair

FTR:  I was going to start that way but I could see issues with getting all the other holes in the right places.

Also, and you can try this with my file if you like, I could not get the centre of the Boss to be coincident with the Origin.  All the verticals were constrained vertical, and the horizontals constrained horizontal.  Concidence with Origin would have pretty-well made Figure 1 fully constrained.  Couldn't get it.  Gave up.

[rickduley]

Thanks for that.

I cannot figure out how you set the two dimensions I have inserted as derived dimensions.  All these holes are positioned in relation to other holes.  It was because of those that I did the layout grid.

How did you set those dimensions?

[JDMather]

Here is my attempt.

[blair]

A simple Off-set work plane from the Origin would solve the creation of the LH Boss.

[JDMather · Accepted solution]

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@rickduley wrote:

....  I resolved the problem by resorting to an AutoCAD technique which is laying out a dimensioned grid (Sketch 1) then outlining according to that (Sketch 2). 

Thanks

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Here is a comparison of your Sketch 1 & 2 and my Sketch1.

Note that you have not located the origin at a logical location - I located at the datum for most of the dimensions.

(I thought we covered the BORN Technique in some detail previously?)  (I did cheat a bit on that though - as I should have used the bottom machined surface as a datum.)

Note that you have repeated dimensions - I guess if you like doing extra work....

Note the dimensions circled in red are incorrect.

[johnsonshiue]

Hi! If I were you, I would consolidate features as much as possible. It should be possible to just create 4 sketches (one for XZ view, one for YZ view, and two for the Ribs). Then share the sketches to create necessary features. Also, as a good practice to ensure feature editability, try to create fillets as the last group of features when possible.

Thanks!

[JDMather]

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@johnsonshiue wrote:

..... It should be possible to just create 4 sketches.

Thanks!

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I used a 5th sketch to cut away cast material that I had added for the purpose of better fillets.

Since the part is machined from a casting....

[PaulMunford]

I just wanted to make sure that the OP has seen this :

http://resilientmodeling.com/_4-Inventor.html

[rickduley]

Thanks Paul, but I get 404d when I try that link.