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I am practicing with Inventor LT 2021 to get used to it, and learn more about how to manipulate things in it. I was practicing with the following sketch and I developed a bunch of questions about the sketch.

Practice Sketch

I can see the thickness of the main plate is 11 (noted just to the left of the overall 65 dimension for depth).

  1. How do I position this main plate in terms of depth from the reference plane to the near face of the plate? I see a dimension that looks like 51 but that makes no sense to me as it mean it would be beyond the back face of the lower or left circles which are 38 (19+19 or 24+14) from the reference plane.

  2. Is is safe to assume that the arm going from the middle to the upper circle has its back side flush with the front side of the main plate? Or is it notched/stepped in slightly? Is the back of the upper circle flush with the back of the arm?

  3. The main plate is 11 thick, and the upper left circles are 14 thick. Assuming this was centered on the main plate that would 1.5 overhang each side. The general fillet note states R2 fillets. Is it possible to place an R2 fillet in that space? I was not sure if fillets had to be tangent to their mating surfaces.

  4. At the back edge of the center, left and lower circles is a V mark. I am assuming this has a specific meaning in the machining/mechanical engineering world. What does the V mark mean? no fillet? (I come from the structural/bridge engineering world so not familiar with most symbols for parts)

  5. When drawing something that has a tolerance to it such as the left ream hole 14.27 - 14.32, what size should it actually be drawn at in the model? I have been picking a nice number that is within the range then navigating to the tolerance for it and entering the max value and the minimum value.

I know if I was in an office I would go ask the engineer/designer/client for clarifications, but since this is just a practice sketch from an PDF online I don't have the source to ask.

This is what I have so far:

Status

For those wondering why I have not accepted my previous question, I am planning to as soon as I work my way back to that question and try it again with some of the new techniques I have learned by stepping back by more than a few examples.

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    $\begingroup$ There are too many questions in this question. IMHO you need to break down the question and focus a bit more. $\endgroup$
    – NMech
    Oct 5 at 9:07
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I'm answering your direct questions in this post, and will follow up with a how-to-model as a separate answer.

  1. How do I position this main plate in terms of depth from the reference plane to the near face of the plate? What looks like a "51" is actually a "5" and a line, dimensioning the depth of the hidden detail cutout (a mirror of the notch on the front of the part)

  2. Is is safe to assume that the arm going from the middle to the upper circle has its back side flush with the front side of the main plate? I wouldn't say it's safe to assume this, but I agree with your assumption. If in doubt, ask whoever you are making the model for (I realise this doesn't apply to your practice use case) Is the back of the upper circle flush with the back of the arm? Yes, I think so. There is not a sharp corner callout on that top circle's back face, suggesting that the back edge of the top circle is coincident with the vertical edge. Likewise, no dimensions indicating any setback means you should assume colinearity where it looks to be that way (in the same way as tangency is implied elsewhere)

  3. The main plate is 11 thick, and the upper left circles are 14 thick. Assuming this was centered on the main plate that would 1.5 overhang each side. This is not a good assumption - if it were centred, then there would be an 0.5mm gap between the 27 wide arm and the main plate... The general fillet note states R2 fillets. Is it possible to place an R2 fillet [a space <2mm] Yes, this is totally fine. The 'white faces' will have been post-machined after casting, so it's expected that the 2mm fillet has been partially removed.

  4. What does the V mark mean? no fillet? Correct.

  5. When drawing something that has a tolerance to it such as the left ream hole 14.27 - 14.32, what size should it actually be drawn at in the model? You should pick the 'nominal' size of the tool to be used. In this case, for the 14.27-14.32mm hole, this will be a 9/16th Inch reamer (yuck). I would model the hole to be 9/16 inches. (14.2875mm...) Likewise the 12.67-12.75mm hole is for a 1/2 inch reamer.

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I'm modelling this in SolidWorks, because it's what I have installed on this PC. Everything should be transferrable to Inventor, but ask if you have any questions.

Step 1 - create the central core. N.B. the '8mm' here is a driven dimension. The drawing shows 8, not 8.0, thus I'm inclined to thing the marked 8mm is a rounding error. Placing the hole concentric with the centre of the R9 makes much more sense, and would still give 8mm on the drawing for that dimension if set to 0DP.

Step1

Step 2 - Create the Circles. I say create these next, since they are the functional geometry. The webs/joints between them are driven by these. If the design were to change, you want the webs to be late in the tree. Note the reamed diameter has an equation =(9/16)*25.4) to accommodate the inches problem. I have sketched on the front plane, and defined the 24mm offset starting position for the extrusion in the extrude feature. Having all the sketches on one plane will make the webs a bit easier to define, without as much 'projected geometry'.

Step2

Step 3 -

Repeat Step 2 for the other two circles.

Step3

Step 4 - Cut the 8mm hole in the bottom right cylinder. In order to avoid creating extra reference planes that aren't needed, I sketched this on the Right Plane, and defined the cut to start 'from vertex', picking up the centrepoint of the sketch which defined the cylinder, and then 'up to next'. This will dynamically rebuild to be cutting from the right place, to the right distance, regardless of how the model changes.

Step4

Step 5 - Extrude the 'arm'. This is defined by literally three dimensions, and the implied tangency and collinearity stuff that I mentioned in the other answer.

Step5

Step 6 - Extrude the main plate. Note that the R51 is not concentric with the central core... This is defined as 11mm, starting from the back of the arm.

Step6

Step 7 - Add fillets. I had to do this in a few steps in order to get the best looking fillets - order of operations matters. This is a whole 'nother topic/answer in and of itself, so I'm not going into it here...

Step7

Step 8 - Realize you've forgotten to cut the notches. Don't forget there is a mirrored copy just visible via hidden detail on the original drawing. This is that '51' dimension again...

Step8

Step 9 - Admire your work.

Step9

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