Vertical and Horizontal constraints not working

[AlexanderYates]

Hi,

I've encountered the problem below. My sketches have horizontal and vertical constraints, but as you can see from the measure tool these aren't working correctly as there is a very slight angle between the two vertical lines, where it would normally read "Angle: 0.0 deg". This then throws everything else in the model into a spin.

Is this a bug, or could it be down to my hardware? I was modelling at the time it first appeared on a MacAir (so not exactly great for doing what are fairly complex sketches and modelling!), but the problem still exists when i open it on a more powerful PC... i've done the full uninstall and reinstall, and the problem hasn't gone away...

I can't share the whole model for confidentiality reasons, but as the problem exists in the very first sketch, i can delete everything thereafter in the timeline and send it on if anyone is willing to take a look?

Any suggestions?

Thanks,

Alex

[HughesTooling]

If you can copy the design, trim it down to share it would help a lot. One thought, is there a line under either of the lines, if you click on the line and hold do you get a selection dialog?

Mark

[HughesTooling]

This looks suspicious, horizontal\vertical constraint icons are normally at the line midpoint. It could be the box with 2 is covering the icon for line 2 but I'd check line 2 has a constraint. 

[AlexanderYates]

Hi @HughesTooling,

Thanks for having a look at this. I've attached the file with the sketch in it. There's quite a lot going on in there as it drives the majority of the model.

It doesn't seem that there are 2 lines overlapping anywhere, and the vertical constraint does seem to apply to that line, although as you say it isn't central....

If you'd be kind enough to have a look that would be much appreciated, as i'm a bit confused as to what to do other than to go waaaay back and start from before the error occurs...

Thanks,

Alex

[HughesTooling]

After drawing another line I know's vertical, the problem line is the one labeled 2 in the image below.

One thing I notice in your sketch is you have a lot of collinear lines, the problem one is in a chain of 4 or 5. I deleted all the lines and drew one new one then added back the constraints and dimension and it worked fine, there is  a bug but all those chained constraints is not doing you any favours. I don't know if you know this but Fusion slows down when there's a lot of info in a sketch so it would be a good idea to use one line rather than chains of collinear lines if possible, try the extend tool rather than adding a line.

I've attached your file 

Mark

[AlexanderYates]

Thanks @HughesTooling

Yeh i see what you're saying with the collinear, i never really use the extend tool, so i'll start doing that. The sketches get quite broken up as i chop and change them, so given what you've said i clearly need to go through and tidy them up. Thanks for taking the time to have a look.

Do you think this a bug that's caused/exacerbated by working on an underpowered laptop?

Thanks,

Alex

[HughesTooling]

The computer you're working on will not affect the accuracy of the sketch only the speed. The best advice is to keep the sketch as simple as possible, just replacing those 5 lines with one removes 4 vertical constraints and a coincident from each end, repeat that over the whole sketch you'll remove 50% or more of what's going on calculating the relationships between all the constraints. If any of the arcs you have in the sketch are for fillets on the extruded part leave them out of the sketch and add them as a feature from the modify menu.

Mark

[AlexanderYates]

Thanks Mark @HughesTooling

This is really helpful to me, i didn't realise that about the arcs either, so i'll just have to go through the model and perform a bit of a clean up exercise. It'll teach me to be a bit tidier with my sketching in future!

Do i need to report this to Autodesk then if it's a bug? 

Alex