Drawing Sketch Error

[khriswright]

When creating a drawing for a component in the model, I need to added geometry via a sketch to aid in manual machining at 45deg angles.  In this model, drawing DrawingError shows two dimensions with warnings. The dimensions reported by Fusion is WAY off and cannot be trusted.  Unknown where these dimensions are coming from but dimensions using added sketch geometry is NOT reliable.

[jhackney1972]

Please indicate the model sketches you are referring to.

[khriswright]

This is a drawing environment issue, sketch in a drawing, drawing is named "DrawingError"

[jhackney1972]

You did not attach a drawing to your post.  Please do so if you need help with it.

[khriswright]

I am not sure I know how to do that other than sending a PDF.  I cannot find a way to send the file, I did include the project in the initial post. Let me know how to get it to you.

[jhackney1972]

The video will  show you how to export the drawing and the model as a file which you can attach to your post.

[khriswright]

File attached

[jhackney1972]

That is one crazy sketch you want to dimension but I see no problems with it.  I will agree that your drawing does not function properly but I created a new one, after updating your model sketch a bit, and it seems to work just fine.  I am sure I missed a dimension as the sketch makes not sense to me anyway.  The model and drawing are attached in ZIP format as the Forum seems to have issues accepting a F3Z file. 

[khriswright]

Just so you understand why I need to create drawings of this magnitude, I do not have a CNC mill to lean on.  This extensive dimensioning is to allow me to machine these features on a manual mill using a rotary table.  In order to do this, I need coordinates for all features (even fillets) that are aligned to std XY and 45deg coordinates.

This is why I need the drawing sketch to work properly, to this point, I have NO confidence is adding a sketch in a drawing environment.

[bwalker145]

The dimensions with warnings are pulling from the sketch that you added in the drawing environment, and not the model itself (two different scales).

I hid the drawing sketch (sketch 3) and re-associated the dimension, and it looks to be correct now.

Best practice is to create the sketch within the model itself (instead of within the drawing environment) if you need to reference it in your drawing.

Edit: Just to illustrate the point, change your model scale from "3" to "1", and you should immediately recognize the issue.

[khriswright]

Thanks for your reply. I now understand how the drawing sketch works in the drawing environment, but I will throw it out there that this makes no sense.  If I am working on a drawing at a 3:1 scale the sketches should also be at that scale (or 1/3 in this case). I cannot always dimension drawings at a 1:1 scale!!

You mentioned creating these dimensions I need in a Design environment sketch, this is what I had to do and print them as a JPG.  Is there a way to get design sketches or none body features into the drawing environment??

[bwalker145]

Yes, you can display the sketches made in the Design environment onto your drawing. After you place a view, just navigate through the browser tree to the component that the sketch was built under, and then toggle visibility both for the "sketches" folder, and the specific sketch that you want to show. You can also change how the sketch looks via "Document Settings" (color, line type, width).

I won't comment on the utility or purpose of the Drawing Sketch function, as I haven't found a legitimate use for it. My guess is it's tied to the scale of the physical sheet size, and not the component views, which causes the discrepancies. Other issue is the Drawing Sketch isn't constrained to the views, so if you create a sketch and then move the view, the alignment will be off. This is where building the sketches within the Design environment come into play, as it maintains the association with your actual model. Same idea as creating joints to assemble components vs. using the "move" function to locate.