Angled dimensions/alignment

[john.n.johnson]

I built a rapid prototype out of wood using the drawing dimension (see exported file of the model) and find that the alignment for the holes of the 3 aluminum supports which connect the 3 panels are off by approx. 0.525" with respect to aligning the top and bottom panels with the angled panel. To show the position of the holes on each panel, I created drawings for each panel with its associated aluminum support, printed these on transparency paper and used them as a template for the hole positions (see one example attached). 

In addition, as part of the wood build, I cut the panels to the lengths and angles per the drawings and found that the lengths of the top and bottom panel were off (longer). Which I had to re-cut to fit.

I am obviously doing something wrong. Something I don't understand.

Any help/guidance is greatly appreciated.

[etfrench]

Simply Extrude components 5 and 6 through the Z components, then Combine/Cut them from the Z's, but keep the tools.  If  you are CNC'ing it or 3d printing, the Z components are done.  If you are manually drilling the holes, then create a sketch on one face of each Z component and Project the body to the sketch.  This will give  you accurate locations for the holes.

[john.n.johnson]

Thanks for the update/input. The issue I have is that I need to be able to accurately dimension along the angled line from the tip to the center of the hole (see attached image). I have tried all the dimensioning selections but non provide the "angled" dimension. I did try to go into the drawing sketch mode and selected the inspect function, but the numbers when compared to the drawing are not accurate (off by almost 1/8th of an inch). Is there something I could do to get an accurate dimension along the angle. 

Many thanks once again.

[jhackney1972]

Here is the dimension you requested.  The two edge points line up as illustrated by the extension line so the applied dimension is the same.  This is a unconventional method of dimensioning the lower hole. If you need an explanation on how it was created, just ask.

[etfrench]

Did you actually try to extrude/cut/measure?

Note: Just add the radius of the hole to the measured distance.

And if you don't want to do all of that, just measure it in Sketch2😀

[etfrench]

But if you really need the distance from the end of the angled plate to the center of the dowel, then do the extrude/cut/sketch/measure routine:

[john.n.johnson]

Hi John, if one constructs this as a triangle, I am looking for the dimension of the "hypotenuse" which comes out to 3.56", when using a triangle calculator. I use this dimension to create a transparency template to mark out exactly where to drill a hole on the angled piece which perfectly aligns with the hole on the horizontal piece. However, I would like to determine this dimension from within Fusion 360.

Hope this makes sense.

[etfrench · Accepted solution]

You have all of the information needed to determine that in your sketches.  The position of the three columns are shown in Sketch2 and the angled plate edges are shown in Sketch1.   Simply draw a vertical line in Sketch1 offset from the left vertical line a distance equal to the horizontal position of the column.  Trim the line to angled line representing the angled plate.  Measure the distance between that endpoint and the left vertical line.

If you create a sketch on the face of the angled plate, you can then project the center of the column from Sketch2 to that sketch.  Project the body of the plate and then use the sketch to create your transparency.

[john.n.johnson]

Thanks for the detailed explanation/illustrations. I did do the extrude/combine per your earlier e-mail. What I got hung up about was getting the dimensions from the center of the circle/hole.

Many thanks for the excellent/timely support.

[jhackney1972]

I believe this is what you asked me for.  I think you realize, this dimension can be taken from the model sketch but this is the way to locate it in a 2D drawing.  You create an auxiliary view and use a model sketch point to establish the center.

[etfrench]

When you print the transparency, make sure it comes out 1:1.  Fusion 360 is notorious for printing 1:1 at 93%😒