How to attach these sketches

[sprior913]

I'm trying to design a sizing gauge for woodturning which shows a min/max tenon size.  I'm trying to keep things very parametric so I can make a few of them with different sizes and I've created user parameters for the size of the openings, the length of the neck between them, and the width of the piece around those dimensions.

At first I tried drawing this as a single sketch and had problems attaching the second side to the neck with the midpoint of the side to the midpoint of the neck.  Then I tried drawing each side and the neck as 3 different sketches, but don't know how to alighn and attach them together.  I want the midpoint of each end to attach to the midpoint of the ends of the neck.  Of course if I change the parameter for the length of the neck it should all adjust accordingly.

Can someone give me the step by step instructions on how to do the final move/align/attach constraints?

[sprior913]

I exported the design to a f3d archive file, but when I try to attach that to this post I get an error that the file contents don't match its file type.  I guess I've got two questions now - how should I attach the design to this questions?

[TheCADWhisperer]

My guess is that you need to Project Geometry from one sketch to another and add appropriate sketch constraints.

To attach a file here, first right click on the filename and select Send to Compressed (zipped) Folder and then attach the resulting *.zip file.

[sprior913]

Here's the zip file.

[TheCADWhisperer]

Editing your Sketch1

- I don't see any Horizontal or Vertical constraints on any of the lines?

- I don't see any size dimensions except for arc radii.

- I would use Equal (=) constraints rather than repeated dimensions.

- It is usually better to add fillets as features rather than as sketch entities.

Q1. Do you have a compelling reason to add the fillets in the sketch?

- I see a lot of symmetry in Sketch1.  I would use this symmetry about the Origin Center Point.

Once I know the answer to Q1 - I can demonstrate how I would create Sketch1.

[sprior913]

Thanks for your help.

I'll be the first to admit that I'm early in the learning curve for CAD tools (despite having a long history of playing with them) and haven't found much "best practices" guidance, so the way I'm doing things is my best guess on how it should be done from the available documentation and looking through the menus.  Given that I think like the programmer that I am instead of a CAD expert I probably do fall for things that appear to be the right way of doing something, but are a blind alley.  I also haven't found a lot on how to properly set constraints.

I created this design by first entering the dimensions I need as named user parameters, so later when I was creating the lines I would fill in the parameter name instead of a numerical length, and used 90 degree angles everywhere so things should be square.

This is the second iteration of this object, the first had incorrect dimensions and I hadn't used parameters and had too much trouble trying to figure out how to modify the existing dimensions.  In that first drawing I did the filets on the model instead of the sketch, but when I did it again I thought maybe doing the filets on the sketch was the way it was supposed to be done, apparently I had it right the first time, but could you explain why?

[sprior913]

We probably got distracted by the update, but I'd still be very interested in some guidance on how to do this.

[sprior913]

I took another shot at drawing this from scratch and setting constraints.  I think I'm closer, but now can't change some of the user parameters because I get an "over constrained" message, but I can't figure out what constraints are causing the problem or how I can delete them.  When in edit sketch I tried clicking on the constraint symbols, but they don't seem to be selectable.

The user parameters that I can change are:

max_length

hole_diameter

min_depth

max_depth

The user parameters I get an error when I try to change are:

min_length

width

neck_length

Can anyone suggest how to determine which constraints are getting in the way and how to remove them?

The other question I have seems simple, but I couldn't see the correct way to do it.  If I start with a line A, how can I draw line B with a length C such that the center of line B is at the end of line A and the two lines are perpendicular?

[NicolasXu]

Hi,

I checked the file, it seems there are two fixed point in the sketch, which causes the over-constrained problem. It’s a known issue related to the fixed point that Fusion should have reported warning when adding dimension instead of changing dimension.

I also attached a new sketch I created based on your file. Using 90 degree is fine, but I would prefer to use Perpendicular constraint because it would keep the sketch clean & in most cases Fusion can infer such constraint during line creation. Also, if the lines are connected and collinear, I would prefer Extending the existing line to reduce the number of sketch objects.

For the selection issue of constraint symbols, at present the selected status is not so easy to distinguish (It’s a little different between selected and deselected). We already be aware of the problem and working on a resolution.

As for the last question, I would create Line B with a length C first, during the Line B creation, I can easily infer the Perpendicular constraint to Line A. After that, I would invoke Constraint command, and then select Line B and end point of line A to add Midpoint constraint. 

[sprior913]

Thanks, I'll look at your file.  I don't understand how during line creation to just specify a perpendicular constraint and not the 90 degrees - can you explain how to do that?

As for my line A and B question, the situation I'm referring to is from this drawing where I started drawing from the left opening to the right and had the center line for the neck in place, but then needed to add the piece on the right perpendicular to it.  So I don't think it's always practical to draw line B first and then line A coming out of it.  When you redrew my sketch what procedure did you use to attach the second side to the neck?

[sprior913]

How did you determine that there are 2 fixed points in my file?  I can't find them - is that the little lock icon constraint?  I'd like to understand if my drawing was fixable or did I need to start over?

[NicolasXu · Accepted solution]

Hi,

I just realized that you might input & lock both length and degree during line creation. If it’s the case, the inferred constraint will be ignored because user-input value has higher priority.

I have recorded a video to explain how I check the over-constrained issue, and to answer the Line A and B question. Hope it helps, please let me know if any questions.

https://screencast.autodesk.com/Main/Details/1b90abad-7284-4108-8616-9b480cd2912f

[sprior913]

Thanks for that screencast - it expanded my knowledge of Fusion 360 a lot.  I think I need to practice a little more, but have a much better understanding of the process now.