Not sure why this explodes so much.

[MattJobson]

Hi,

I'm a longtime solidworks user who is still transitioning over to Fusion. I've spent most of the day trying to look for answers to this issue searching here and youtube and I just can't figure it out.

I'm having issues with projections and intersections not updating dynamically when parameters change. I tried to create a file to show the main issue, but found I was creating an explody mess before even getting to the main issue. So I must be doing something really bad.

I've uploaded a file to show what I must obviously be doing wrong.

I'm used to creating a master sketch to control global sizing, then (for simplicity and ease of selection) creating sketches on top of that master sketch where I add more detail.

In this files case. I have a master sketch, then on my 3rd sketch I offset the master sketch in 2 directions and create lines between the intersections to be used to split the main body into individual components.

(I actually tried to split the bodies at the bodies intersection without relying on the sketch, but when that had issues updating I tried to control it with a sketch. I also tried to project the intersections into the sketch, but ended up going for real sketch features, but even this doesn't work)

I then split the bodies. I even chose to do them individually because I thought that might help.

Everything works fine until you start to adjust the 4 parameters I made.

The file shouldn't explode into a mess just by changing a few paramaters. I never even tried to give it numbers that would deliberately cause it to explode (eg. numbers smaller than the diametre of the tube in length etc)

What am I doing wrong here? This technique would work 100% of the time in Solidworks and never present an issue. To me this is basic functionality and I just don't get what i'm doing wrong. 

I've made many very detailed multi-scalable configurations in Solidworks that rarely ever see yellow or red, but Fusion it's like I set off a bomb or something.

Please help.

Kind regards,  Matt Jobson

[davebYYPCU]

I've uploaded a file to show what I must obviously be doing wrong.

Not obvious.

The Split bodies using a remote cutter, need the extend option to be ticked.

Can't see what you want to do,

At this stage there is nothing showing where the outer ring of bodies created / originated / arrived on scene.

Need a few clues.

[MattJobson]

Thanks for the quick reply, but I sent the file after it exploded and created double geometry. My point was to show the extra unexplained geometry and all the red and yellow.

If you look at the original sketch I only want 1 enclosed tube that can scale in length, width and angles. But when I try to do that it has all sorts of issues.

Also, the extend splitting tool option, what is the purpose of it other than to save time and as a quick fix if you didn't already draw the full line you want to split? I found it would get int the way and split things I didn't want it to.

[laughingcreek]

you have a lot of symmetry that will simplify the sketching.

offset is sometimes buggy

mirror is sometimes buggy

using both together, idk?

you can have more than one split tool in a single split command (that functionality may be newish, not sure)

sketch 3 not fully defined, may be source of problem.  would be helpful to have the model BEFORE it explodes, and then the steps that make it explode to understand problem.

attached is how I would approach what I Think you want.

[MattJobson]

Thanks Laughingcreek.

I tested your file and it works much more robustly.

I have read that sketch patterns in Fusion aren't very robust yet. Is that the case for Offset and mirror in sketching too?

I did oringally have more than one split tool in the single command, but to try and reduce the issue I made one command per split. It didn't make it better.

This is only the beginning of the issues I'm having. The file i sent was an overly simplified version of the main file I am working on. (which I can't send due to IP)

I do have mostly symmetry in 1 direction, but I have a lot of external components where the joints are failing and some internal components where the entire drawing flips when I scale the model up a down.

This is frustrating, as it takes a long time to basically open up each issue and respecify a joint snap point to a sketch intersection.

I've attached a screenshot of the main issue.

On this tube design there are a lot of external components that need to attach to it. Was it stupid of me to:

1. make a sketch with a bunch of dimensioned lines on it,
2. that are controlled by custom parameters,
3. then make construction planes at 90 degree angle to the tube,
4. then create a sketch on that construction plane and create an intersect of the tube, then close the sketch,
5. then create a joint where I snap the external component sketch to the tube intersection sketch

Is there a better way to achieve the same result? Because when I scale up and down all I get is a random exploding mess.

I guess some of that mess is caused my my sketch features, but i'm wondering if there are other causes eg. the intersect sketches?

Sorry this is long and sorry I can't send the main file.

[davebYYPCU]

1. No.

2, that's Ok, (provided the sketch is fully defined)

3. Why? go to step 5

4. Why? go to step 5

5. Use the supplied snap points.  Every cylinder has a centre snap and two end point snaps.  Use the Joint Offset function (it's parametric) to get to the required (step 3) position.

Scale Tool ignores Parameters, so if you mean changing Parameters to change something, OK but if you mean Scale the document - dont do that.

Might help....

[TrippyLighting]

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@MattJobson wrote:

Thanks Laughingcreek.

I tested your file and it works much more robustly.

I have read that sketch patterns in Fusion aren't very robust yet. Is that the case for Offset and mirror in sketching too?

---

I would not necessarily believe everything you read online!

Offset is indeed not a very robust implementation. Extruding surfaces and working with surface offset creates more reliable designs.

Patterns and mirroring in sketches are to be avoided or at least reduced to a minimum. That is good design practice in all parametric CAD software, not just Fusion 360. 

[laughingcreek]

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@MattJobson wrote:...Was it stupid of me to:

1. make a sketch with a bunch of dimensioned lines on it,
2. that are controlled by custom parameters...

...Is there a better way to achieve the same result? Because when I scale up and down all I get is a random exploding mess.

---

many many issues addressed here on the forums trace back to sketching.  it's always a good place to start looking for problems.  I have found many times that using a bunch of custom parameters with equations etc. will trip people up because it's rather easy to create conflicts that way.   OTOH, you can do some interesting things with that approach, so sometimes appropriate.  personally, if I can represent it in a sketch visually I will.  I find keeping things working (and find errors when they aren't working) to be much easier to deal with than combing through a bunch of parameters in a table.  the primary thing I will create a custom parameter for is quantities for patterns and things like that.  when I do create other custom parameters, I keep it to a minimum. (and make a comment about them so I can remember why a year from now when I open the project again!).

so with that said, it may be worth it to repost the original example in a working condition, and then give us a change that makes it break.  that will help in understanding your problem better.

did you look at sketch 3 and see what I mean about it not being fully constrained?

to echo what has already been said-

I don't ever use mirror in sketches

I keep offsets to a minimum.  it works ok on lines and arcs mostly, sometimes can be problematic sometimes not.  never on a spline. 

i try to do most of the sketch definition with constraints,  then add dimensions as necessary. 

[TheCADWhisperer]

@MattJobson 

CSWP since 2007 here.

Robust sketching is the same in any history based parametric CAD software.

Simplify Sketch1

Alternative

[MattJobson]

Thanks everyone, I appreciate all the help and advice,

@davebYYPCU I've taken on board your advice regarding removing construction planes and sketch intersections. However I really wanted to just snap to the line (but seems I can get the same result using parameter names in the offset field, but it lacks that visual connection. I clicked a line that I want to constrain to and I want it to stay connected when I scale it. The parameters and even when you change that input field to d42, it just feels like a total disconnect, but i realise it's the way the sofware works)

I appreciate what @TrippyLighting, @laughingcreek & @TheCADWhisperer have to say regarding correct sketching techniques, however I would counter argue somewhat that you should be able to get away with basic functionality of pattern, mirror, offset, even fillets and chamfers in sketches.

Everything I did on that super basic model would work 100 % of the time scaling up and down dimensions in Solidworks, Onshape, Siemens NX, Solidedge.

Yes it's a dumb idea to create anything more than a super basic pattern in a sketch, it's dumb to put all your fillets in a sketch as you can't remove them without a lot of editing, it's dumb to have a complete mirror of a sketch if you have no further use to reference it later. But I counter that there are occasions where a little bit of each in a sketch can greatly reduce feature complexity, but it often can increase errors.

I'm trying to understand how best to proceed forward, but I am struggling to figure out what it is I am doing exactly. If mirror is a bad idea, then is the symmetry constraint a bad idea?

I just feel like i'm being told "you're doing it wrong" but I can't for the life of me figure out how to do it right. haha

I wish someone did a direct video on that.

I removed all the IP from the main file i'm working on and I've attached it to this reply.

But i'm stumped on what I should do to fix this file. I know that when I make a major dimensional change (eg. switch configuration from "current" to "default") that the sketch "split bodies" fails and breaks everything else.

But I get the sense that it's not just the split bodies sketch that is the issue. It's also the 2 sketches before it, "tube Path" and "Master Sketch"

If anyone could help me see what it is that I'm doing exactly that causes split bodies to detach from the projected curves from Tube Path? (When I projected them, I had "projection Link" ticked)

This is causing all the features and sketches after it to be flipped or lose references. Now i'm fine to fix them, but I want to make a configuration of 20+ different sizes and styles and it can't explode like that every time you switch configs. And the reason I'm building both sides is because there is asymmetry in certain areas.

I know i'm doing it wrong. But what specificially? Thanks.

[jeff_strater · Accepted solution]

I understand what is going on here.  It looks like a bug in Fusion.  The projected geometry is updating just fine.  You can see if you just change Boat_Width to 5000:

The projected curves are correct (highlighted below):

What is NOT correct, though is the offset.  The offsets have lost their connection to the projected geometry, which is why they do not update, and why the sketch shows as failed.  I have a theory about why this is - sometimes, if the changes are big, projected geometry is re-created instead of just updated.  Because those new curves have a new identity, the offset cannot find them.  I suspect that all of your other problems flow from this one.  This is partly why people are recommending to tread lightly on symmetry and offset.  In this particular case, symmetry works OK, but offset fails.  I agree with you, you should not have to avoid features like symmetry or offset.   This bug should be fixed.

In the meantime, you might be able to get away with a trick:  Use Offset to create the offset (to prevent the tedium of manually creating the offset), but then, delete the offset constraint.  This will try to convert the offset geometry into "regular" geometry, with distance dimensions to the source curve.  You might have to add some parallel constraints, etc, but I suspect (though I have not tried it) that this might be more stable for you, until this bug gets fixed.

It's late here, but I will create this Fusion bug tomorrow...

[MattJobson]

Thanks Jeff. Appreciate your candidness. And thanks for the trick. I did try deleting the offset after a few people mentioned it was problematic, but it immediately gave 100 dimensions and i gave up.

I should i played more with constraints. I'll do that now as stopgap. Thanks again to Everyone. It was all valid and useful advice. Much appreciated.

[davebYYPCU]

I would like to help, but you have me intrigued, 7 cutter lines, and 14 bodies from only 3 Split Body commands, each having only one cutter selected.  No mirrors, no patterns.  How did that happen?

Next you are still saying when I scale it.

What are you doing to make the file break?  It is not broken as received.

Edit: Wrote this reply before seeing Jeff's response. 

That said, why do you need the offsets at all?  A?. (I need to see it)

[MattJobson]

I feel like the split body command needs to show a list of selected lines/planes etc that were used.

Also it feels a little buggy that "sometimes" when you edit that split body feature it shows only 1 cutter, when the first one should show 2 and the second should show 4 cutters, and the 3rd should show 6 cutters.

Sorry for my use of the word scale. I'd NEVER actually try to haphazzardly scale the whole model (actually that probably wouldn't have broken things LOL)

When I was saying scale, I meant changing the main driving parameter values or dimensions. I did say in the last message that changing the configuration from  "current" to "Default" would cause it to explode.

And this time I did provide the file un-exploded (un-broken) and like above listed a clear step to break it.

But it's all good. Because @jeff_strater gave me a great trick to get by while they look at fixing the bug that caused it. And i've managed to impliment it and prove it works consistently!

Thanks again to everyone! 

[laughingcreek]

the split body did seem buggy here, but didn't investigate further than the sketches.  wondering if that clears up once the sketching is sorted.

FYI, tons of way to get a bisecting angle other than offsetting.  this is one of my preferred ways-

  but have used many others.

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@MattJobson wrote:......I did say in the last message that changing the configuration from  "current" to "Default" would cause it to explode.

And this time I did provide the file un-exploded (un-broken) and like above listed a clear step to break it.

...

---

the file you uploaded doesn't have any configurations.  but it was easy to break non the less.

[jeff_strater]

I created bug FUS-143676 to track this issue.  Thanks again for reporting it.

[MattJobson]

Thanks Jeff.

The theory you mentioned yesterday,

" I have a theory about why this is - sometimes, if the changes are big, projected geometry is re-created instead of just updated. Because those new curves have a new identity, the offset cannot find them. I suspect that all of your other problems flow from this one. "

I kinda hope that theory isn't true, but I was working on this model until 3am this morning and noticed similar behaviour with some much more complex sketches in the design. They weren't using offset, pattern, symmetry, but were heavily using projections. And if I try to resize an overall dimension the whole thing just falls down. haha

I even had a bunch of cases where the part was working without errors, but the sketch had the projections all in green instead of purple and other than deleting the projections and redoing it, there was no way to re-reference. But at the same time it wasn't reporting an error.

I'm just going to roll with it and try to only do global changes at the start of the job.

[laughingcreek]

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@MattJobson wrote:... but the sketch had the projections all in green instead of purple and other than deleting the projections and redoing it....

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green means the "fixed" constraint.   (confusingly the padlock in the constraint toolbar).  if you redefine the sketch plane for a sketch, all projections get removed and have the fixed constraint added instead.  did you happen to redefine the sketch plane?  if not would be good to find out what causes those to become fixed so the coders can work on it.