Extrusion doesn't match sketch dimensions

[mlitzkow]

OK, I must be doing something stupid, but this just seems wrong. I'm modeling a "Circle Diamond Square" which is a classic test cut for a CNC machine. Some in the forum probably recognize this object. I made the model two different ways, but in both cases the measurement of the extruded "Diamond" part seems to be off from the dimension of the sketch object it was extruded from. The official description of the object and the dimension in my sketches is 26.52mm on a side. However the extruded diamonds seem to measure 26.513mm. Both of the sketches in question are fully defined. I am including my Fusion 360 file. Please tell me why I am not getting the size of part that I expect. 

[jhackney1972 · Accepted solution]

I believe you got in trouble using Construction lines in the creation of your inside rectangle.  Take a look at the same sketch in the attached model.  I used the midpoint of each side, of the larger rectangle, for the corners of the smaller rectangle.  This avoided the slight error in your sketch.

Edit: If you measure from side to side, of the opposite faces of the small rectangle solid on your model, you will find one measure shows a very small angle.

[mlitzkow]

I don't see an attached model, so I can't look at what you are saying. However, the specification I was given says the sides of the "diamond" part (really a square placed on an angle) are to be 26.52mm. Whether those corners reach exactly to the midpoints of the surrounding square is not something I know. That's why I defined the lengths of the sides and didn't use the midpoints as you describe. It seems that I have those sides of the diamond dimensioned clearly, but the sides of the extrusion (as shown by the "measure" tool) is different. I am hoping you can tell me why that is, and how I can correct it. I can't change the definition of the object, that's a given. The drawing I'm working from is here: https://www.researchgate.net/figure/Design-of-the-circle-square-diamond-part-a-simplified-embodiment...

[jhackney1972]

In the video I point out where you go in trouble in your sketch.  The Midpoint of the side of the large rectangle is just a little under 25.52mm so when you sketched, you got off by that small amount.  This introduced a small angle between two faces of the small rectangle model.

Model is attached.

[mlitzkow]

You are quite right John. Many thanks for your help. I have accepted your solution.

[g-andresen]

Hi,

Here is another simple way to create the sketch.

günther

[mlitzkow]

I'm sorry, but it looks to me like this video illustrates the problem, not a soution. Look at 1:12 in the timeline. The "measure" tool says the line is 26.5165mm long, but I need the line to be 26.52mm as specified in the drawing I referenced earlier. The problem here is that the points of the triangle shouldn't match up exactly with the square, but it's very easy to accidentally get them lined up in your sketch. Figuring out how to avoid having Fusion make the incorrect assumption that the diamond points should be on the square is the real issue. However, thanks for looking at and responding to my problem.

This may seem like a very nit-picky difference, but the object I'm modeling is used for calibration and comes from the NAS 979 standard.  This small difference is important in this case.

[g-andresen]

Hi,

1. Please reply directly to a post and not by quick reply (in this case to yourself)

2. If the inner square is to have an side length of 26.52 mm and all corners are to lie on the sides of the surrounding square, the outer square cannot have an side length of 37.5 mm.

günther

[TheCADWhisperer]

---

@mlitzkow wrote:

The problem here is that the points of the triangle shouldn't match up exactly with the square

---

@mlitzkow 

Just to clarify - is it your true Design Intent to have these four corners of the second square outside of the first square?

[mlitzkow]

If the inner square is to have an edge length of 26.52 mm and all corners are to lie on the edges of the surrounding square, the outer square cannot have an side length of 37.5 mm.

The sketch I'm working from doesn't say that the corners of the diamond coincide with the sides of the square. As you point out, given the other dimensions, they can't. The crux of the problem was creating the sketch in a way that avoids introducing such an (erroneous) constraint.

[davebYYPCU]

Disable the auto constraint system, with Cntrl or Cmd key being held down during the sketching process.

If splitting hairs, the drawing has 2 decimal places, which means both measurements are correct, 

.5165 will be .52 to 2 places.  Yes Fusion is that accurate.

Might help….

[g-andresen]

Hi,

perhaps this procedure will help

günther

Correction

at 0:44 it has to be 26,52 instead of 26,25

[davebYYPCU]

Try 26.5165…..

[mlitzkow]

Just to clarify - is it your true Design Intent to have these four corners of the second square outside of the first square?

Yes, as you say, the corners of the diamond fall outside the square. I didn't design this object. It's comes from NAS standard 979 that's used for calibration of CNC machines. I'm just trying to use the darned thing, and it hasn't proven easy so far. This "feature" makes the object fairly difficult to sketch correctly in Fusion, but as we've seen, it can be done.

I haven't actually set up the CAM for this object yet. I had been assuming that the corners didn't match, but would fall inside the square. Now I see, as you have pointed out, that they fall outside the square. So, how am I going to machine that on a 3-axis machine? Certainly not in a single setup as I am pretty sure it's intended to be used. I will have to cut off the silly corner overhangs anyway. That's not the part that gets measured in the end, so it won't make a difference, but it seems pretty goofy to specify it that way.

OK, I'm going to back up here. The standard is publicly available, so I downloaded the whole thing and perused some of its 60 pages. It's considerably more complicated that the simple drawing I downloaded earlier. In fact the original specification is in inches, not millimeters. I'm not going to study the whole thing - I'm just a hobbiest wondering how accurate my machine is. The idea of using an object with this shape is good. For my purposes I could alter the dimensions by a small amount and still meet my purpose as long as I compare my measurements to the actual part I model. I don't have to certify the machine - I just want to use it effectively. This has been quite a learning experience - both about Fusion and the naieve use of standards.

In case  you're wondering... The original standard shows 5 significant figures. Since we're dealing with 45 deg right triangles, there must be a factor of the square root of 2 in the dimensions of either the diamond or the square. The square root of 2 is an irrational number. If you assume the corners of the diamond should meet the sides of the square, the 5 significant figures can only be taken as an approximation. The document is copyright 1969 and I guess nobody saw a need for more than 5 figures on that. That's way more than enough for my needs, but using it with modern tools like Fusion certainly took me down a rabbit hole...

Again, thanks to all the forum members who have contributed to my education today!

[davebYYPCU]

Change your preferences to measure to 2 decimal places, 

the drawing you published requires the diamond to align to the square.

Might help…..