Rectangle pattern - What am i missing?

[doncawley]

Hello, I am modeling a workbench I will be creating and am having trouble in the sketch creating the proper thickness from parameters.

From the images attached you will see that I am attempting to make the cross support a thickness of 1.5 ( all my pieces of steel in my frame are 1.5x1.5 ).  I am finding the proper position of the cross support by drawing a construction line between the opposing corners and then using the rectangular pattern tool to make two lines half the thickness of the material from that construction line.  So I input " SteelOD / 2 " which should translate into 1.5/2 = .75 which would then properly create two lines 1.5 apart.  However when I complete the pattern and measure, it shows the two lines are 1 19/64 apart.  

I can't for the life of me figure out how or why this is happening.   It might have to do with the " distance type " attribute but its in two dimensional space with infinitely thing lines, so I don't think that would matter; plus i think i tried both choices.

I imagine there are other ways for me to complete the model, but I have a bunch of different parts attributed to this sketch and while I am interested in better ways for the future, i would really appreciate any help or input as to how to fix it as is.   Thank you!

[doncawley]

attaching actual file if needed.

[etfrench]

The rectangular pattern is moving horizontally and you're measuring diagonally.  Attach your file for more detailed analysis (File/Export/Archive file *.f3d).

[doncawley]

Interesting!  I would have imagined the toold would calculate distance perpendicular to the source line.   Thank you for pointing that out.  Are you aware of any way to solve my problem?   I assume it would have to be done with setting constraints instead?

[etfrench · Accepted solution]

Attached is the file with a sketch the way I would draw it.  Note the sketch is fully constrained and the frame is centered on the Origin.

[etfrench · Accepted solution]

Rectangular pattern is the wrong tool to use for this.  Offset is the correct tool.  You can use Rectangular pattern, but you will need to add a direction line.  In this case it would be at 90 degrees to the pattern line.

[doncawley]

If i understand your file properly, you just created an offset line at 3/4 on either side of the construction line, correct?   Yes, that would absolutely work if doing that from the start.  I guess my mind screwed me over thinking i could be more effectient trying to only do one move instead of two.   Thank you!

If you are aware of a solution that I could edit from, it would be appriciated.  This sketch is the basis of a more parts in other models and is dupped in this model too.  I would really like to avoid having to a whole bunch of extra work if needed.

[etfrench]

I think it would be best to bite the bullet and redo the file from the start using fully constrained sketches.  It goes pretty fast when you already have the design.

In Fusion 360, moves and aligns should be avoided as each of them need to be recomputed each and every time a change is made.  They may be used then deleted after creating a joint. 

I would also only model one steel tube. Use Copy/Paste New to create modifiable copies or create an external copy and use Insert/Derive.  Position them with joints.  This allows you to easily change dimensions and have the entire model updated.

When you have symmetry, use mirroring or patterns.