How To Trim While Keeping Sketch Fully-Defined?

[Anonymous]

Y'all,

I was critiqued by @TheCADWhisperer for many of my sketches not being fully-defined, particularly Sketch10 of the accompanying file.  As attached, said sketch is fully-defined, but when I begin trimming to eliminate the internal arcs, the geometry becomes under- or un-defined.  How would one trim this while keeping it fully-defined?  My intent is to have the radii of the corners concentric with the circles on the other sketch and eliminate the extraneous geometry internal to the perimeter of the rounded-off rectangle.

Alternately, what technique(s) would be better for creating the concentric corner radii that I'm trying to end up with?  A rectangle with fillets of the desired radii?

Thanks,

Shawn

[TheCADWhisperer]

Is Sketch1 fully defined? No? You are building on a shaky foundation.

Are all sketches in sequential order fully defined. No? Getting shakier as we go.  I am starting to experience vertigo...

Tip: Often it is not necessary to trim sketch geometry.

Tip: I recommend starting over from scratch using what was learned from initial attempt rather than trying to put lipstick on a pig.  The darn pig won't cooperate...

Tip:  As you are modeling an assembly of parts - be sure to find information on Components.

[Anonymous]

You have my assurance that this piggy is headed to the rendering plant and has already been hit with the bolt gun.  However, this cosmetologist would like to examine the corpse before the remains are sent off.  It's educational to know where the makeup smeared before simply starting with a zygote.

FWIW, this is not going to be going into an assembly of parts -- it will be stand-alone.

[TrippyLighting]

To stay with the metaphors, this piggy was DOA.

Not constraining and dimensioning sketches in any mechanical design is a pretty bad idea, particularly for people new to the field.

In general, there is no reason to trim anything in this design. In Fusion 360 You can extrude several sketch profiles at once and if they are adjacent the resulting bodies will auto-join into a single solid.

This can make more complicated sketches hard to read. But there's no reason to create more than one sketch. In general I move from sketch so solid geometry as soon as I can.

[laughingcreek]

You are also wrestling with a bug in the sketch engine.  I know sketch 10 looks fully constrained (as uploaded, before trying to trim), because all the lines are black.  But it's not.  You can tell because there is no push-pin icon on the sketch in the browser.

I'm able to repeatably get the circle in the upper right quadrent to turn blue or black, depening on the sequence of what I click on.  Definitely a bug.

@jeff_strater, can you look at this probable bug?  I can screen cast if you need.

[Anonymous]

Thanks, @TrippyLighting.  To respond to a few things:

"Not constraining and dimensioning sketches in any mechanical design is a pretty bad idea, particularly for people new to the field."
I wasn't arguing otherwise, wasn't taking any position on it, and am not averse to it.  I simply didn't grasp the significance of it -- that's all.

"In general, there is no reason to trim anything in this design. In Fusion 360 You can extrude several sketch profiles at once and if they are adjacent the resulting bodies will auto-join into a single solid."
I do understand extruding functions that way.  However, extra unnecessary bits make the piece look cluttered, and if it's possible to inadvertently overlook some teensy piece such as the wedges formed by the overlapping circles in my example above (or an inadvertently created new body as per my other post I linked above) I want to eliminate that as much as possible.  I'm not new to modeling and believe it's good practice to minimize the number of elements, especially if they're not performing any real function -- that's my main intent in trimming.

"But there's no reason to create more than one sketch. In general I move from sketch so solid geometry as soon as I can."

I was not aware of that design philosophy -- I will look into that.

[Anonymous]

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@laughingcreek wrote:

You are also wrestling with a bug in the sketch engine.  I know sketch 10 looks fully constrained (as uploaded, before trying to trim), because all the lines are black.  But it's not.  You can tell because there is no push-pin icon on the sketch in the browser.

I'm able to repeatably get the circle in the upper right quadrent to turn blue or black, depening on the sequence of what I click on.  Definitely a bug.

@jeff_strater, can you look at this probable bug?  I can screen cast if you need.

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Ah, thanks for that, @laughingcreek -- I was getting pretty confused by that.  I was finally able to trim in a different order and get it all cleaned up with no blue lines left, but since I am going to be doing the entire thing over anyhow, that was really just some experimentation/practice.

[TrippyLighting]

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@Anonymous wrote:

"But there's no reason to create more than one sketch. In general I move from sketch so solid geometry as soon as I can."

I was not aware of that design philosophy -- I will look into that.

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Something many people that are new to CAD have difficulties with - I am not saying you do - is to dissect a part they see and want to model into it's elemental pieces of geometry. tThey see the whole and are overwhelmed. They do not see the pieces it's made up of and also cannot relate the pieces to the CAD tools these can be created with. That usually takes a little practice.

While I've also come across sketch bugs, I try to keep my sketches simple. I don't put any purely cosmetic fillets in my designs, ever. I evaluate what symmetries are present in a part so I only have to model 1/2 or 1/4 or sometimes 1/8 of it if possible.

[jeff_strater · Accepted solution]

@laughingcreek and @Anonymous,

I understand what in going on in Sketch10 in this model.  There are two coincident circles in the upper right hand side of this sketch.  One is dimensioned, which makes it fully constrained, and the other is not.  That's why the whole sketch is not fully constrained (no push pin in the icon).  You can see this if you use Select Other (hold the left mouse button for 1/2 second), you can see the existence of the two circles.  And, if you rotate the view a bit, you can see them "z fighting" with each other - sometimes you can see the pink (under constrained) circle, and sometimes you see the white (fully constrained) circle.  One of those items in the Select Other list is the under constrained one.  Select and delete it.

Jeff

[Anonymous]

Another nice catch -- thanks, @jeff_strater!

[dieselguy65]

i understand the deisre to trim sketches. i do it myself on any that have alot of geometry.

sure makes it easier when you start extruding them into 3d bodies.

trying to find each little segment to select gets old really fast.

i have missed more little corners and pieces than i care to admit.

as long as my sketch, before trimming is fully constrained, i dont really get myself to concerned with the warnings.

might be and probably is bad practice to ignore them. but it makes the sketch simpler, and future operations so much easier by cleaning it up.

[TheCADWhisperer]

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@dieselguy65 wrote:

i understand the desire to trim sketches....

trying to find each little segment to select gets old really fast.

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I have been using various CAD programs for 30yrs.  

I am supremely confident of sketch trimming skills.

I never ever have little segments left over.

Having established that baseline of experience - my experience of trimming sketches in Fusion I would describe as maddening compared to other parametric MCAD softwares.

Other than missing functionality - certainly my pet peeve in "existing" functionality.  I would encourage the Fusion team to "walk across the hall" and talk to their Inventor co-workers.

You might start the discussion here.

[dieselguy65]

i think i used some wrong terminology, or was misunderstood

i mean if i draw a square, and put lets say two tangent circles in the corners.

now to extrude that into a solid i have to select the middle section, then each circle. if i trim the inside portion of the circle on each corner. i make one selection, and extrude.

much cleaner imo

[ericdlaspe]

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@dieselguy65 wrote:

i think i used some wrong terminology, or was misunderstood

i mean if i draw a square, and put lets say two tangent circles in the corners.

now to extrude that into a solid i have to select the middle section, then each circle. if i trim the inside portion of the circle on each corner. i make one selection, and extrude.

much cleaner imo

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That certainly makes the sketch look cleaner and makes the extrude operation easier.  When it removes constraints, however, you may end up with a problem if you need to resize any part of your design.  

I like to make my models both fully constrained and use as many named User Parameters as possible so that I can change any value in the Parameters dialog and the design's geometry will all be recalculated correctly. I know exactly what to expect from changing any dimension. When trimming removes my constraints, not adding them back is not an option, and adding them back is always a pain, so I avoid trimming.

Does anyone have tips for maintaining constraints or easily adding them back when trimming?

[TheCADWhisperer]

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@ericdlaspe wrote:

Does anyone have tips for maintaining constraints or easily adding them back when trimming?

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@ericdlaspe 
Another option is to use Break rather than Trim and then toggle the geometry to Reference.

I use this often.

[ericdlaspe]

Break is an interesting tool I hadn't used before. I just tried it, but I don't understand what you mean by "toggle the geometry to Reference." I was able to successfully break a circle into arcs and make one of the arcs into a Construction line. That's nice since it keeps my constraints. Is that what you mean?

[TheCADWhisperer]

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@ericdlaspe wrote:

Break is an interesting tool I hadn't used before. I just tried it, but I don't understand what you mean by "toggle the geometry to Reference.”

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Yes.

Rather than Trim away geometry,Break it instead and then right click on the geometry you would have otherwise Trimmed and set it to Construction.  In some cases you might lose a Constraint, but usually fewer lost Constraints using Break rather than Trim.