Should it be this hard? (to constrain a sketch)

[davethomaspilot9V8SL]

I'm trying to take the advice of prior posts and take the time to constrain ALL my sketches.   Maybe it's because I'm not that skilled in F360, but I'm struggling a lot to figure why something isn't constrained and how to constrain it.

A screenshot of my latest struggle is below along with an exported model.  

The radial line segments that connect the arcs are constrained to be co-linear with the origin.

The radius of the outer arc is dimensioned.  The difference between the inner and outer arcs is dimensioned.

The inner holes geometry won't move and everything behaves as I expect when change dimensions.  The holes extrude Ok.

I was advised (I think) to avoid using circular pattern in a sketch and use Create Pattern from the Solid Design workspace.  But, I couldn't figure out how to select the holes for a pattern repeat.

What am I missing?  It's taking WAY to long to figure out to constrain my sketches.

[jeff_strater · Accepted solution]

sometimes it is very hard to do this, and sometimes there are bugs.  But, one technique I use a lot is to just try to drag things, and see what moves.  It will often be obvious where the degrees of freedom are.  ESC to cancel the drag.  In this case, you can see in the drag that the angle of the ends of the slots are not constrained, so I added 2 angle dimensions.

[davethomaspilot9V8SL]

Thanks!

It never occured to me to try dragging versus trying to move everything.  But it makes sense.

The type move I was trying was a default translate.    I didn't think to try a rotate move.

But, dragging is a good tip.

[davethomaspilot9V8SL]

What do you do to get an dimension in degrees instead of linear?

I did it once, but can't figure out what I did/ need to do to repeat.

[davethomaspilot9V8SL]

Finally got it.

[davebYYPCU]

We recommend new people gain an understanding by making one sketch per modelling feature.  They become very simple sketches to constrain.  You have too much detail for quick modelling, in that one sketch.

I don’t have access to the file, it appears to have 4 circular discs, and 2 hole patterns.

I would likely have revolved the disc from one profile.

Top view sketch would have one hole of each pattern, as a neat pie segment.  Then extrude Cut the hole of each ring.

Now it is easy to circular pattern both holes in one feature, set the pattern type to Feature, and select the Extrude Cut icon off the Timeline, set the centre axis and count.

Might help....

[laughingcreek]

different approach.  you can see I was pretty lazy with the second sketch.  also patterned the feature instead of the sketch objects.  primary advantage to that:1-less sketching 2-changing the number of thru slots is just a matter of changing the parameter "num_of_slots" (if you leave the patterning in the sketch, you'll have to go back and manually edit the extrudes to add the profiles)

question-why is this located so far from the origin?

[davethomaspilot9V8SL]

I'll give it a try again. but I couldn't figure out how to select a hole.  I did have object type "Features".

[davethomaspilot9V8SL]

question-why is this located so far from the origin?

It was created and exported from a larger model that contains it and several other components.

Origin is at the center bottom.   The lid component is over 28" away from the origin.

It is not used by any other model.  It's just standalone/exported for attaching to the post.

[davethomaspilot9V8SL]

Interesting...

Note that your sketch is not fully constrained 😀.  Took four more dimensions to fully constrain.

I've been dutifully adding dimensions to lengths of lines whose lengths really don't matter.  Seems especially silly for construction lines.

T

[laughingcreek]

like I said, got lazy with the sketch.  shouldn't take anymore dims though. see attached