Which point am I projecting?

[Anonymous]

I sometimes need to intersect a line or a curve with a construction line to indicate a spot on the geometry where I want a place a drawing point. Fusion terminates the construction line with a little circular point. If I place a point on the geometry, it will snap to the point on the end of the intersecting  construction line, so I'm guessing that I'm now placing one point exactly on top of another. If I later tell Fusion to project the point, which point will  it use?

If I delete the construction line after projecting the point, would this explain the error message I sometimes get that Fusion has lost the original point and is using a cached location instead?

I guess you could call this a Cache-22 situation? 😁

[TheCADWhisperer]

If you do a long left click on the entity when in Project, you will get a "select other" list that will permit you to select the intended entity.

[etfrench]

Break the link before deleting the construction line to avoid the error.

[Anonymous]

Sorry for the long delay in responding. I've been trying to clean up some things in Fusion first before further annoying you guys, but the program has been chugging along very strangely. spinning blue wheels and the browser screen going black for considerable periods even after very simple things like drawing a line or placing a drawing point. Not sure how to make it go away, but at least I'm getting more familiar with the rabbit hole.

Thanks very much for your advice. This is a really neat (and needed) feature that I wasn't even aware was available. I'm not secure yet in what actually happens when you click on a selection under the "depth" tab, so a little more explanation would be welcome. Believe me, every little bit is a great step forward for me!

[Anonymous]

How does one break a link, or be sure that the link being broken is the intended one? Just once I saw a "break " choice on the mouse-click menu, but I was in the throes of a newbie meltdown and so far have not been able to get it back. It looks like one of those things that only appear on the menu under specific circumstances. If you can clarify what those conditions are, I would be embarrassingly grateful.

[davebYYPCU]

For Sketching, 

Break Link will appear in the Right Click Menu, If the article you have selected is actually linked elsewhere at the time.  Projected articles are purple, (in my colour scheme) they are the linked articles.  When you select the purple article the Project icon appears near your cursor, selecting that icon instead, and then deleting it will do the same job.

Might help....

[Anonymous]

Can you (or anyone else browsing by) take this drawing and delete the construction lines in such a way that it remains fully constrained? The explain how you did it as if I were six years old? 😐 I have not been able to call up the break link option you told about, so there's obviously a disconnect somewhere on my end. Using the long left click and having Fusion cheerfully point out that it sees two (or sometimes more) sketch lines is not helpful. I already know there are two sketch lines!  Resolving this will probably clear up at least half the problems I have.

[etfrench]

The Break Link option is only valid when you project something.  This doesn't appear to be the case here.

Why do you want to delete the construction lines?

If it's just because of the clutter, then simply start a new sketch and project the geometry you need.

[Anonymous]

Yes, it is because of the clutter and partly because once the outline is complete, the construction lines are no longer needed. Unfortunately the lines are necessary to create the drawing. When I delete the construction lines, I lose the fully-constrained state of the sketch because Fusion applies the dimension points to the construction line and not the drawing line, and I don't know how to tell Fusion which line to ignore. 

Specifically, the points will next be used as terminations for arcs in intersecting planes, which is when the points get projected. Here again, I need Fusion to go to the drawing lines, not the construction lines. Otherwise it can lead to error messages in lofts. Damned if I do, and damned if I don't.

 If it helps, the construction lines are draw first. If Fusion maintains a display order, the drawing lines would be on top.

[davebYYPCU · Accepted solution]

This may help, https://autode.sk/34c25yC

All the Construction lines can be deleted without penalty, but you have to remove the dependencies first.

They are two of the lines that are coincident to the end point of the large radius, as pictured.  There are duplicate vertical lines there, so I got some small grief from the sketch solver, when I add the dimension, but stop and restart the edit was ok for that.

[Anonymous]

I was only expecting a relevant, but nevertheless generic, video addressing my complaints. If you had been a fly on the wall and could have seen my face when I looked at your screencast and saw my sketch, well, I suppose imagining a laughing fly would also be pretty funny, too! This video just completely got me over the hump. I was able to go back to some of my earlier attempts and successfully delete the construction lines while still maintaining the sketch's fully constrained state. Then I was able to make some changes and re-constrain the sketch fully. Huge step for me! I also picked up some useful concepts about using radii to help constrain a sketch if other  constraints and linear dimensions were removed. I can't thank you enough for your time and assistance.

Having reached a new plateau, of course I am pressing remorselessly onward since I need to do further work on this sketch. And, naturally, I am encountering exciting new mysteries because this is Fusion after all. The first of these might be easy to explain-- I'd just like to know what Fusion is trying to tell me if a sketch dimension turns red, and why as I scroll it back into view after working elsewhere on the sketch, it has sometimes turned black again.

I've attached my most recent effort, which I'd love to finish because it would complete the 2D part of the sketch. As you can see, in the upper portions the lines are still blue, and I would understand that they are not fully constrained. After plugging away at it so much that my sketch dimensions and constraints look more like a pot of badly petrified spaghetti, I shut down last night so I could upload it this morning. The puzzling part is that no matter how I attempt to constrain the blue lines, Fusion tells me that the sketch would be overconstrained! Not sure what's going on here.

Hope your experience will make short work of this one without using up much of your valuable time. And thanks again. Happy Camper here.

[davebYYPCU]

Pleased your pleased.  Some comments in no particular order. 

I was not able to constrain your sketch, not enough info, or too many guesses needed, (without the known detail you have).  The blue articles in your supplied file sketch have lots of white dots (first sign of problems)

some curve overlaps (- found where the white dots are).  Select a curve, the highlight shows which end point is associated.

I could rebuild a sketch, with a method I picked up in threads here along my way.  

Tackle any job by breaking up into small modules.

Quick check - I found one curve set that can be offset to both sides,  to supply a quick 3 track sketch.

1.  Constrain as you go.

2.  All constraints you can before dimensions.

3.  Use flexibility when using these 2 points.

Summary of what I did, 

Build and dimension away from the Origin, (arrow)

top horizontal line, is also the first radius.

Use dimensioned construction line to trim that first radius, (1) then added 3 Tangent Arcs about the right shape, dimension the arcs, then I dimensioned to the origin, point 2 in the photo., then the centre points of the intermediate curves, when locked will fully constrain those 4 curves.  (3)

So the rest of the curves consisted of two sets of 3 curves that are tangent segments, 1 - 3 point curve and use Tangent Arc tool to make the next 2, then dimension them.  Dimension the last end point of the 2nd set, and the centre curve's centre point.

We now have 6 black curves.  So now another 3 curves, (guess 1), same method,

Due to the lack of info in the first sketch, I dimensioned the end point of the first curve of this set, and that got them to turn black.  Ideally that point should not be the one carrying the dimension, but I did not get enough info to lock the 2nd curve's centre point.

With nine black curves, I then Offset the inside.  18 black curves.

Offset the outside, all black but the second point can't be a point, so fusion filleted it.  Those two flat portions are a later addition.

Last thing, top neck area, (not shown), 2 lines, vertical / horizontal, and dimensioned, when adding the Tangent arc, made tangent to both ends, doesn't need a dimension.  

So now there is just the two waist lines to go.  (warning - do not trim the offset curves - will break the sketch)

When you get this far, you may figure it out, but will give a few clues if stuck.....

Might help...

[Anonymous]

Thanks again!! I worked late yesterday and was able to fully constrain the sketch after simplifying it a bit, and, I admit it, starting the process from the beginning. 🙄 I think I have discovered that the source of the problem is probably the way Fusion and I handle offsets (meaning, not quite the same way). As you know from my sketches, there is a simple "master" sketch I use as a template, and to get the outer and inner lines I use the offset command. My assumption was that if the arcs were constrained as tangent and coincident, then the offset copies would be as well. The lines were black at first, but lacked dimensions. They also did not show constraints, so I added them. Not sure about this, but perhaps due to bungling when trying to get the lines black again I moved the lines imperceptibly. Enlarging to maximum magnification I could see a second little circle where the lines met just beginning to peek out from behind the first. Not sure why this happens, but in my efforts to trim and butt the ends of the lines together, the sketch broke. I think I need to find a way to correct overlapping lines without making more work for myself.

>>1.  Constrain as you go.

>>2.  All constraints you can before dimensions.

>>3.  Use flexibility when using these 2 points.

I was already coming to the same conclusion, but I was using dimensions first more than constraints, I know I can constrain a sketch like mine using tangent constraints; would using coincident at the same place be overkill?

>>Build and dimension away from the Origin

Yeah, buddy! If there were a Fusion bible, this should probably be the first commandment.

Nothing needs to be done on the attached file. It's just for your information. I do notice that on the mirrored side there are tons of mirror constraints, but no others and no dimensions. Looks like an accident waiting to happen, doesn't it? OK, I am off now to get myself into more trouble, but also much better equipped now to deal with it. This has been an excellent exchange. I owe you a beer, but for now I hope my appreciation will be enough.

[davebYYPCU]

Yep just a little polish, (other than that file's extrude is broken)

Another chapter in your bible, fix broken timeline icons when they happen, good chance you did it in the last operation, next month you wont remember why you broke it.

Why mirror? 

Looks like an accident waiting to happen, doesn't it?  NO.

Trust Fusion to mirror for you in the modelling areas.  Sketch > Mirror askes Fusion to work twice as hard for no obvious result, the sketch solver has more chance of breaking / slowing down, (further down the track, the centre helper body for the crown is required, so mirror the bodies is inevitable.)

However, when you mirror a sketch,

the no dimensions and no constraints is wrong, bit, 

is not right, Fusion has swallowed all the original dimensions and constraints, and delivered them in a summary of mirror constraints. 

Same for sketch Offset, offset a chain of articles, and they are black, - sweet, job done, (black is black, how easy was that?) is don't touch or you get blue nightmares.  If offset won't chain, there is a missing coincident.  When Offset does chain, one dimension swallows all the other construction under the hood, and delivers the summary in the offset icon.  Delete the icon, you get blue nightmares again.  You been there this is why.....

Cheers

[Anonymous]

>>Another chapter in your bible, fix broken timeline icons when they happen, good chance you did it in the last >>operation, next month you wont remember why you broke it.

I hate those things. I see the yellow glow of pain in the timeline and (very faintly) hear in the background, "ha-ha-ha. Bet you have no idea why this happened". Fixing is still a hit-or-miss affair with me, but never one that's postponed.

>>Fusion has swallowed all the original dimensions and constraints, and delivered them in a summary of mirror >>constraints

I think you mean a flood of mirror constraints, sometimes so many that I can no longer see the line they reference! But it does explain why all the others are absent. One of a number of odd things I noticed is that when I am trying to intersect a point, I get a visible indication of success on the original side, but not on the mirrored side, even when I attempt it separately. Also, I have wondered whether the point should turn red (or whatever color) if the project / intersect succeeds, or if it should be a circle of color around the point. It happens both ways to me and I don't know why that is unless Fusion is just catching up.

>>don't touch or you get blue nightmares. If offset won't chain, there is a missing coincident. When Offset does >>chain, one dimension swallows all the other construction under the hood, and delivers the summary in the offset >>icon. Delete the icon, you get blue nightmares again. You been there this is why.....

I have been there, and I was just visiting that same place again this morning. I appreciate knowing that I should be looking specifically for missing constraints. I changed one thing on my contrabass sketch this morning, and the entire drawing turned blue. "Eff it", I said, "I'll deal with this later." I kept on with my work drawing intersecting planes and arcs for my arching lofts, and little by little the drawing turned black again. Not touching it again! (Sound familiar?)

One other strange thing happened, but I think I'm going to put that in a new thread on the effects of precision. Have a happy thanksgiving!

[davebYYPCU]

I kept on with my work drawing intersecting planes and arcs for my arching lofts, and little by little the drawing turned black again. Not touching it again! (Sound familiar?)

Nope.  Not seen that, but that would be cause I know why that happened, intended or not, and fix it as I go.

…. to intersect a point, I get a visible indication of success on the original side, but not on the mirrored side, even when I attempt it separately.

I get a visible indication of success on the original side  - red preview, and purple surround on a black dot, on confirmation.  Means the black dot is fully constrained, and the purple surround is - it's projected.  All correct.

.

.. but not on the mirrored side.  The Intersect command does not chain, so it will do both sides for an ellipse or circle, but not separate splines.  The mirror keeps track of the selected articles, move one article in the mirror the other side updates, but a new intersect point is not part of the running mirror.

even when I attempt it separately,  Do you mean pick either spline the other doesn't work, or pick on the mirrored side and it doesn't work?

I did this screencast to show a reliable workflow for Loft rails, and first time lofting, last week, see if this helps....

Not my file, and was finding the intersection connection errors, few thinking pauses but we get there....

same processes, different shape.

Might help....

[davebYYPCU]

I kept on with my work drawing intersecting planes and arcs for my arching lofts, and little by little the drawing turned black again. Not touching it again! (Sound familiar?)

Nope, likely because I know why it happened and restore it, before moving on....

when I am trying to intersect a point, I get a visible indication of success on the original side, but not on the mirrored side, even when I attempt it separately.

I get a visible indication of success on the original side, yes, red dot is preview, confirm and you get the black point and it's purple outline to show - Projected.

but not on the mirrored side, After a mirror, a new point is not in the mirror, Intersect does not chain, but if an article crosses twice, (ellipse and circles) it will produce 2 points, but separate splines are one at a time.  Was hoping to cure you from mirrored sketches by now....

even when I attempt it separately. Not sure I got this bit...  pick either side and it wont select, or doesn't do two at a time, as above...

I did this video last week, same problem, repairing rails not connected, first time loft is a normal workflow, similar to Jeff's series.

https://autode.sk/2D0LL8f

Might help....