What am I doing wrong?

[MattJobson]

Hi, I've been dealing with a bunch of annoying issues on my main CAD files for months now. So I decided to try and start again from scratch. I made sure not to use the mirror or offset commands in sketch and It's still not playing nicely.

I'm completely stumped now. I've attached the new file I started.

If I modify the parameters "Boat_Length" and "Boat_Width" the bottom surface doesn't resize/scale/move (pick your terminology) with the top surface. I've supplied it broken. 

Set "Boat_Length" to 5000 and it lines up again. Then set the length to something smaller. (eg. 3500) and no issues. Now set it bigger (eg. back to 5000) and it fails again. HAHAHAHAHA MADNESS!

Also, the split body command. You have the option to select multiple lines to combine splits in the command and it will split the amount of bodies you ask it to (eg. select 2 bodies to split 10 lines as splitting tools). This will work, but immediately after that right click and edit that split body feature to find only 1 splitting tool is selected????

This is why I added 12 split body features. I thought that might be casuing my problems, but no it isn't.

I really don't know how to move forward from here other than spending most of my day redefining features that I have defined hundreads of times already and while I like a lot of the features of configurations I can't take advantage of them when my models fall apart every time I change a length or width. (my actual workaround has being doing it in small incriments. LOL)

Can't anybody pinpoint this? Can anybody help me to make robust models in Fusion?

[Warmingup1953]

Have you investigated and attempted to resolve the yellow highlighted?

[laughingcreek · Accepted solution]

lets look at the sketch "floor flap profile"

here you have 2 arcs of regular line type (as opposed to construction line type) laid over the top of each other.  Not the direct cause of your problem, but is bad practice for a variety of reasons.  it's fine to lay a regular line type over a construction line though.  In this case you are obscuring your issue making the problem a little less discoverable.  so lets change the larger arc to a construction line type-

and then change boat_length to 7000

The problem is a little more obvious now.  the large parameter change is causing the way the angle is dimensioned to change reference directions.  This is an issue with the sketch solver.  can't tell you why it happens, but is a fairly common problem with large changes in values.  we have to come up with a different way to define the arc.

changing boat_lenght back to 5000, I created an angle using the same variable you used, but put a vertical constraint on one leg.  then drew a cord between both angles and made them equal.-

now the model doesn't break when you change boat_length between 5000 and 7000

model with above change made to it attached.

p.s.  working way to hard. model half the boat (half the sketching) and mirror the solids after.

[MattJobson]

Thanks @laughingcreek,

This issue was in that sketch. There was only meant to be 1x arc, 1x line with tangent relationship and 3x construction lines. I don't know where the 2nd arc was that you found. It wasn't in my file? Also, due to the issue, that line up the top wasn't supposed to be there. See how the sketch was meant to look like.

3x construction lines

1x arc

1x line with tangent relationship

There was a projection reference that was casuing issues. Once I deleted that, I was able to make a 3000, then 15000 length with no issues.

Deleting this actually fixed it????

This is what the working version looks like now.

Just to be sure, I actually went back to undo changes up until before I deleted that reference line. And it failed... But wait, I tried again to double check it and it worked WITH the reference line, Then it didn't work, but then one final time and deleting the line because i didn't need it anyway, and it works..

I kinda wish I had honed in on this bug now, because with no signifant changes, it's randomly working again. I feel like I am rolling a dice when I use fusion. 😞

[laughingcreek · Accepted solution]

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@MattJobson wrote:

Thanks @laughingcreek,... I don't know where the 2nd arc was that you found. It wasn't in my file? ...

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projected arc is still an arc. so 2 arcs.  -

highly suggest toggling this to a construction type so you can see what's going on when it breaks (you might want to go over the pics I posted previously again also)-

so is your new sketch working with all the parameter changes without breaking or not?  was hard to tell from your reply.

does the version with my sketch changes work with all the parameter changes?

[MattJobson]

WOW!

Ok, so I moved to Fusion from Solidworks. I thought the projected and intersected curves were some sort of "Special Visual Representation" ONLY. This is why I would create them and never touch them.

In solidworks, every referenced line/curve is the same colour as a regular curve. They are all black. The whole time I was using Fusion I never made the connection that those special coloured curves were still being treated as curves!!

Thanks for that! It could be a huge part of why I've been so frustrated using Fusion. And it makes sense why all the comments were "that's bad modelling practice". I just never thought they were actually curves. I never tried to extrude them and i'd always build over the top of them.

I will no go and open up all my files and turn all projections/intersections to construction!!

Wish I knew this months ago!!!! Thanks again 👍

[davebYYPCU]

turn all projections/intersections to construction!!
And blanket statements like that will cause just as much trouble.

Fusion sketches require projections, to snap to, if and when required.

Might help….