Multiple coincident constraints overlapping one another?

[ipmcc]

If I have a bunch of sketch elements -- it seems especially problematic if I cut and paste polygons in a sketch, but it also happens without C/P'd polygons -- where sketch elements will appear to be in the right place, constrained to the origin in some way, but actually won't be. I'll sometimes have 10+ sketch points overlapping the origin. I want to constrain all of these to be coincident with the origin, but, in the starting condition, some points are, and some points aren't. Here we go:

I thought I was a smart guy: I set my selection filter to "Sketch Points" only, select them all by 'rubber-banding' them, and then I try to add a coincident constraint over all of them. If even one of those points is already coincident with the origin (or if two are coincident with each other), the operation fails (often silently).

I have, over and over, moved sketch elements such that the origin point moves away from the origin, and then I re-constrain each point, one at a time. Sometimes though, the act of moving the sketch element seems to have awful ripple effects that do not resolve even when I re-constrain the point. 

Is there a way to filter selection to unconstrained points only? Alternately, is there a way to say "all points coincident, even if some of them are already coincident"? I feel like I lose notable design time to this problem on a somewhat regular basis.

Surely there must be something simple that I'm missing, no?

-Ian

[TheCADWhisperer]

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@ipmcc wrote:

Surely there must be something simple that I'm missing, no?

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@ipmcc 

Can you File>Export your *.f3d file to illustrate this issue to your local drive and then Attach it here to a Reply?

I suspect that it would also be useful in this particular case to provide information on where you are going with the sketch. Perhaps a picture of something similar that already exists in the real world.

[jeff_strater]

"Is there a way to filter selection to unconstrained points only? Alternately, is there a way to say "all points coincident, even if some of them are already coincident"? I feel like I lose notable design time to this problem on a somewhat regular basis."

No, there is no tool available that does exactly that.  There is a debug tool called Sketch.ShowUnderconstrained that will select ALL geometry in a sketch that is not fully constrained.  But, this will likely cause more stuff to be selected than you want.

In general, you want to avoid creating these "point stacks" if at all possible, for many of the reasons you've laid out here.  Mostly, Fusion tries not to do that with curve endpoints, by reusing existing points instead of creating another point.  But, "center" points (circle centers, polygon centers) are handled differently, and can result in those point stacks.  The method you describe of temporarily using Move to see what is free to move, and then using Coincident to put them back together, is really the only option available.

It would be helpful, as @TheCADWhisperer suggests, to post an example here, and then detail what your ultimate goal for the design is.  There might be more efficient ways to achieve your end goal.

[ipmcc]

I fully understand that "fully constrain all your sketches" and "post an example f3d file" are the de rigeur mantras around these parts. I may be new-ish, but I'm not that green. 🙂 Been using Fusion for about a year now. 

Before I posted this message, I genuinely tried to replicate the problem in a new, from-scratch file that I could post to support this discussion, but after more than an hour of effort, I gave up. So, sadly, no, I don't have an .f3d file that I can attach that shows this particular case. Through that effort, I only ended up with a bunch of new problems.

I described the problem as best I could. If you've never run into this problem in your own use of Fusion, then I'm glad for you! But I admit that it probably means that you don't have experience that would be applicable to my problem. I've run into this problem multiple times, across different assemblies, over multiple months of use, and I usually solve it by starting the design over from scratch, but that's not practical in this case. Coincidence with the origin seems like a 'weak' bond, at best.

My personal best hypothesis is that I add a sketch entity (say 'Y') with some point that should be coincident with the origin, but the software treats it as coincident with the something else (say 'X') that is, itself, coincident with the origin. If X is subsequently moved or deleted, Y's point may stay physically 'coincident' with the origin, but, at that point, it has no explicit coincidence constraint to the origin. As stated, the obvious solution of selecting all Sketch Points and setting a coincidence constraint between those points and the origin does not solve the problem if even a single other point is already coincident with the origin.

I have already tried to backtrack the whole design all the way down to deleting the sketch and starting over, but building it back up from zero just created a bunch of new problems that came from not using the projected geometries from otherwise-unrelated components (that I would prefer not to upload), and as such would not be useful.

I understand that it's frustrating when people to roll up in here saying, "Help me!" but don't provide you with a file showing the specific thing they need help with. That's why I deliberately framed this question in abstract terms that another user might be able to relate to. I guess time will tell. I'm sorry to have wasted anyone's time, I just struggle to believe that I am the only person on this forum to have ever run into this problem, given how often I run into it.

- Ian

[TheCADWhisperer]

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@ipmcc wrote:

 But I admit that it probably means that you don't have experience that would be applicable to my problem. 

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Yeah.

CAD "Golf" anyone?

[ipmcc]

I think the message I'm getting is:

If I want something constrained to the origin, I need to select the origin in the browser every. single. time. or there's a better-than-not chance it's going to be constrained to some other point. 

So. Annoying. Especially in light of how all the best practices advice tells you to home everything on the origin. 

Off to start a stupidly-complex assembly from scratch!

-Ian

[jeff_strater]

I don't need an example design to know how to re-create the problem.  Just using circles, and the Move command, I can easily re-create a circle center point stack on the origin where one of the points is not constrained.  It's part of the reason why using Move is discouraged, and to use Coincident instead.  I was asking about the design only because there may be better ways to achieve your final goal than to have a bunch of polygon centers stacked up at the origin.

[billbedford]

Maybe, just maybe, you need to use more sketches?

[Drewpan]

Hi,

I can think of a couple of ways to solve your problem but probably the best way is to

create more sketches to make things simpler. You said that you have been on the Forum

a while (good) and heard a few things that @TheCADWhisperer has asked for (good).

Have you heard another common couple of comments? "Keep your sketches simple"

and "only try to do one or two things with each sketch". There is also another common

saying - "Sketches are a tool, use the right tool for the right job". Pretty much what

all of these "proverbs" are telling people is that the OTHER tools available in fusion work

much cleaner and more robustly than relying on sketches for everything. A good example

of this is a cube with rounded corners and edges. Sure I could use sketches to create

the rounded sides on four sides and then use the Fillet tools to put curves on the other

sides and corners, but a sketch to do this is messy and harder to constrain. Or I could

draw a fully constrained square, extrude it and use the Fillet tool on ALL my edges and

corners. A much cleaner workflow.

You say that you have multiple polygons that you are trying to constrain to the Origin.

What is the purpose of so may of the objects in the sketch? What are you actually doing

with all of these polygons? Why do they ALL need to be in a single sketch? These are all

questions that we have to ask ourselves when using fusion to design things. While most

of the Gurus do this stuff automagically and don't even think about this stuff any more,

once upon a time they were relative Noobs like yourself (One year is still a Noob, don't

be offended as some Gurus here have been doing this stuff for Decades). Once upon a

time they were pretty much where you are right now in your journey.

My advice to you is have a think about your sketches. Put in enough stuff to do only one

or two things. Don't try to put EVERYTHING into a single sketch. If you need stuff from a

previous sketch, use the Projection tool and only project the MINIMUM you need to

continue what you are doing. One method that may help you to get your pollies in the

correct position would be instead of starting at the Origin, draw the polygon in space,

constrain it in space and THEN select the point at which you want coincident at the Origin.

Do this ONE at a time, not as a bunch. Constrain the first polygon, THEN use Co-incident.

Constrain the second polygon THEN use co-incident. This should ensure that each polygon

the last operation should be co-incident with the Origin and ALL previous polygons should

already be co-incident. You will know they are co-incident because you did NOT build them

from the origin and the selected point should snap to the Origin.

Two fully constrained polygons at the Origin.

Cheers

Andrew

[billbedford]

If a sketch is copied and pasted, any point that had been constrained to a projected point will loose its constraint.  This means that the sketch will not fully constrain, and the unconstrained point will be hidden in a stack of points. The best way I've found to deal with this is to check the pasted sketch for black points and delete the spurious point(s) in these locations.

[ipmcc]

If anyone is curious, I redid the part from scratch, with no projections, and was able to get it to be fully-constrained, but again: I had to redo the entire part from scratch. And now that I'm not using projected geometry (instead using copy/pasted dimensions) I've lost the parametric-ness of it, but I did manage to get a clean export. There's really no problem left to solve here I guess, but if you were curious about the part, welp, here it is!

-Ian

[ipmcc]

Thanks to everyone for the tips. I've got a few new ideas from this thread about how to approach situations like this. I think the core takeaways from the thread are:

• 'Move' considered problematic.
• 'Cut and paste' considered problematic
• Draw shapes away from where you want to constrain them, then constrain them after the fact. (I've seen this advice from multiple YouTubers, but never really understood why until now.)
  • I'm going to just put it out there: I consider this to be a strong UX smell. It's one thing to say that, 'this is the workaround necessary to avoid this problem, given the current circumstances', but let's not pretend this is a good user experience.
  • When I click-and-hold and the drop-down comes up with many "Sketch Point/Line/Arc" entries, why couldn't there be a blue or black dot to indicate whether they're fully constrained or not?
• I would really like more visibility into the document model from the browser, but that's probably because I've worked extensively on graphics software packages throughout most of my career, so I tend to think of things in those terms. I expect I will develop proficiency with the Fusion Python API sooner or later, which may help.
• I don't think this particular case was one of an over-complicated sketch, but the point about more sketches is well taken, and I had started to arrive at similar conclusions on my own. Specifically, I have a lot of cases in my designs, where fasteners are involved, and there will be an inset for the head of the fastener and washer, a cut-through for the shaft of the fastener, and then a tapered inset for the nut, and teasing those three sections apart is consistently annoying.
  • The issue I've had with a plurality of sketches is that the ordering in the timeline becomes problematic. It's one thing to separate functional concerns into multiple sketches, but sometimes two sketches really deserve to be one due to interdependence. 

Thanks again to all!

Regards,

-Ian

[billbedford]

I think you have just described the difference between people who think in 2D and draw things, and those who think in 3D and make things. 

[ipmcc]

I'm not sure what you're driving at. I do both of these things! I never mentioned 2D vs 3D. I feel it should be obvious, given that we're talking about Fusion, that at the end of the day it's all 3D. What are you trying to convey?

- Ian

[Drewpan]

Hi,

In response to your summary.

Move is not problematic, it has a valid use under certain circumstances. The problem

is that some users, and particularly new users, do not understand when to use Move.

One of the most common uses for move with new users is to literally move a body or

component out of the way of their assembly because it blocks their view. This is a

huge no no because doing this forces fusion to do a recalculation that can seriously

affect performance. String several moves along the timeline and fusion recalculates

for EVERY one, even if the last entry on the timeline just did exactly the same thing.

Move can and should be used in very specific circumstances and most people only

learn when this is with experience. The correct way to "move this part out of the way"

is to either use a Joint between two components or to simply turn on and off the

visibility on the Browser Tree.

Cut and Paste are also not problematic when used correctly. The problem, again, is that

some users don't know when that correct time actually is. Cutting and Pasting various

Bodies and Components is reasonably common. Doing so in a sketch is often wrong. A

sketch is ONE of the tools in fusion but many people make them way to complex and try

to do way too much in a single sketch. The issue with sketches are that they are easy to

break, and a broken or unconstrained sketch can cause major problems in a design way

after they were created in the timeline. In many designs a sketch is the base that the rest

of the design is built on, but it is also the "weakest" part of the design in some cases.

When designing, patterns and symmetry are your friend. You should always be looking for

them and incorporating them into your designs. I have seen many newer users copy and

paste all over the place when a simple rectangular pattern or circular pattern would have

sufficed. Similarly the Mirror tool could be used. Fusion software is under constant

development and the tools are quite powerful. Sketches are only one of the tools and you

should use the right tool for the right job. There are many similar tools to manipulate solids

that are also used in sketches, fusion handles these operations on the solids way better

than in sketches. An example, a fillet on a solid will not usually break the model, a fillet on

the same two lines in a sketch will often blow away constraints and break the sketch. 

I agree that fusion does have its issues with the UX. Fusion is also under constant development

and many tools and behaviours have been implemented solely from users like you and me asking

for particular features to be implemented. This does not mean that fusion is just "slapped together"

but it does mean that sometimes there are inconsistencies between features that seem logical

they should be similar but are not. Sometimes a "work around" is just a workable method to achieve

an end result until an issue can either be fixed or implemented by the Devs. They are not all bad,

they have just persisted a long time for some of them. Remember that this is mainly a Help forum

and so the users share techniques that "work" and so these "fixes" will come up time and again.

There IS actually a way to tell if a Sketch is fully defined but it is not always obvious to newer users.

An unconstrained line is Blue, and a constrained line is Black. An unconstrained point is a Circle, where

a constrained point is a Dot. You must actually LOOK for them and they can sometimes be easy to miss.

There is also a Text Command "Sketch.ShowUnderconstrained" that will highlight everything that is

not constrained in a sketch.

From your comment about fasteners and inserts and countersinks I am beginning to wonder why you

are using sketches for these features. If I need to put in a countersunk bolt or screw in a model, I don't

sketch it, I will put a Point in my sketch to use as a locator and then use the Hole tool in the model. I

can set everything I need from that tool. I actually WANT to do the modelling that way because when

I create the Engineering Drawings, they are created from the Model based on actual measurements of

the Model, the sketches are completely irrelevant in this process.

I am a little confused about why ordering of sketches in the timeline are an issue for you. This seems

that maybe your issue here is not managing the timeline properly. There are a couple of schools of

thought about how to manage sketches in the Browser Tree that will directly translate to how they

will be added in the timeline. One workflow chooses to create all sketches as part of the Top Component

so they all end up at the top of the Browser Tree and are easy to locate. Some people do this as a preference

and some do it as a Design Standard. A common issue with this method is that people fail to "Name their

stuff" and so locating what Sketch 234 actually refers to can be a problem. The other common workflow is

to carefully manage the Active Component so that the Timeline remains nice and clean and every sketch

and tool operation remains nicely grouped within each component. This makes it much easier to locate

which sketches relate to which component but doesn't help with the Sketch 234 problem in the Timeline

so it is also encouraged to Name Your Stuff.

I agree that there are times when it is better to group some items together within a sketch. The problem

is knowing when to STOP. If a sketch is becoming too complex, save the sketch; start a new one; project

the MINIMUM you need from the previous sketch; continue on with the sketch.

I haven't tackled the Fusion API yet so I cannot offer any help on your "more visibility into the document

model from the browser". I am not 100% sure what you mean here.

Hope this helps.

Cheers

Andrew

[billbedford]

You said yourself that you had come to Fusion from a vector graphics background. Your sketch shows this, it's messy, confused and appears to be dimensioned in order to be fully constrained rather than to show design intent. 

I've refactored your file to use three simple sketches, each linked to its own part of the design, I've also adjusted the dimensions to use more sensible values. 

[jeff_strater]

I can't improve much on @Drewpan 's response here, but I can add a couple of additional comments to your observations.  

"Draw shapes away from where you want to constrain them, then constrain them after the fact. (I've seen this advice from multiple YouTubers, but never really understood why until now.)"

I have not heard this particular recommendation, I never advise people to do that, and I never need to do it myself.  Sketching in place, for objects like circles and polygons, should always create a point-to-point coincident constraint for the center point.  There are some exceptions.  Move is one of them.  If you Move the center of a circle onto another circle center using point-to-point, it will not create a coincident.  Another is an "accidental" coincidence.  If you create two arcs, say 3-point arcs, that just happen to share the same coordinates for their center points, they will not be made coincident.

"When I click-and-hold and the drop-down comes up with many "Sketch Point/Line/Arc" entries, why couldn't there be a blue or black dot to indicate whether they're fully constrained or not?"

There could be, certainly.  However, that is not sufficient.  It is sufficient at the origin, but for other points, it might not be.  In this example, both points are not fully constrained.  But, that information does not tell you whether there is a coincident (or concentric, for arcs - they are identical) between the two points:

As to why Fusion even allows these "point stacks" to be created at all, that is a long story, much debated early in Fusion development.  As I said earlier, most of the time Fusion tried really hard to avoid these.  Center points, though, are the one are where we allowed them.  Simply because: if you ever want to break apart two circles that actually share a center point, it is difficult, and can cause downstream failures.  Was that the right decision?   I don't know - trading one set of problems against another.  But, to be honest, we have not received all that many complaints about this over the many years that Fusion has been out there.

[ipmcc]

@billbedford Thanks for digging in. First, I want to start the discussion by pointing out that my original file was 'well-formed', in that it didn't have any warnings or errors on the timeline, and the file you posted shows half a dozen steps on the timeline with warnings. And I get it; I don't like doing a bunch of unpaid labor in response to forum posts either, but if you're arguing that your way is better, I'm not sure how exactly I'm supposed to see that.

• Looking at your file I notice that your `Sketch 1` has removed the nut/bolt holes. OK. Sure. Separation of concerns into multiple sketches. I'm not sure what that buys us here, but it's certainly something one could do. 
• I notice that you use a Feature-based rectangular patterns instead of a sketch-based rectangular pattern. How did you decide which to use? They achieve identical results, but, in my opinion, doing the pattern in the sketch makes it much more clear to someone who might come along later, what the intent was. 'Four counterbored holes around the middle'. Whereas, you're putting a single counterbore/hole, and then using a circular pattern of Features to multiply it around the hub.
• This same thing repeats itself with the 2x4 grid of holes going out the arm, except this time with a rectangular pattern of features, not a circular.

I'm not trying to be contrarian here, but I don't see how what you've done is fundamentally better than what I did. I did patterns in the Sketch - I wasn't just copy/pasting things willy-nilly; you did patterns of features in the timeline instead of the sketch. To me, this really seems like a six-to-one/half-dozen-to-the-other kind of situation. What am I missing here? Thanks!

Regards,

-Ian

[davebYYPCU]

Not reviewed any files.

Pattern features (etc, over sketch articles) is highly recommended and eliminates huge sketch intensity.

For those who come along later, would not expect to see sketch patterns.

Horses for courses as you say,  but you were able to compare both.

Might help….

[TheCADWhisperer]

@ipmcc 

Are ready to tackle techniques from a logical perspective?

If yes, we can begin the discussion.