Canvas Disappearing

[docara]

Hello Again

I'm trying to draw a circle over a canvas.

I have 5 holes to reproduce, I have done one with no problem. Now, whenever I try to do another the canvas disappears form the screen.

The canvas image is contained within the component I am using but I am unable to move it around the browser tree to see if this helps 

Any thoughts

Thanks

Matt

[Phil.E]

I'd like to help but I'm not exactly sure how to reproduce this effect. Can you make a video using Autodesk Screencast? That will help to show all the picks and clicks you are making.

Thanks,

[docara]

Hi Phil,

Hope this clarifies things a little.

You will notice the first circle I Right Click that the canvas remains both on screen and browser. The second one the canvas disappears from both the screen and browser and I don't understand why.

Thanks 

Matt

[docara]

ScreenCast didn't appear - lets try again

[Phil.E · Accepted solution]

Thanks for posting that. It's pretty easy to see in your video.

In the first instance, you are editing a sketch that exists after the canvas in time. So the canvas is present in timeline, browser, and screen.

In the second instance, you are editing a different sketch that exists in time prior to the canvas. So the canvas, at that point, does not exist in your design.

Other than that, I think you are over complicating your design.

There should be one canvas, early in the design, and one sketch that has all the circles that belong together. Those circles appear to be related, if not an identical array of duplicate circles. It's best to put them all into one sketch if you can.

I hope this helps. Let me know if you have more questions.

Thanks,

[docara]

Hi Phil,

Thanks for the reply. The order of things - that's makes sense, but why does any reference of the canvas just disappear? Why doesn't it just get hidden by virtue of the light bulb getting turned off?  At least I could just re-enable it and carry on!

Over complicating things yes and no! Unfortunately, I'm just REALLY struggling with the UI of F360, I'm very close on giving up on Fusion completely to be honest (I've come from Acad2007). I just don't get the logic of what the software is asking of me or what it expects from me - even down to command noun-verb / verb-noun selection processes. The user UI is terrible and not consistent across commands. I cant find any information on what is good practices . Yes, there are lots of 'How-To' videos on commands (notice I didn't say tutorial) but no basic information on how to draw with F360 anywhere, no proper help files or informative command feedback prompts on screen.

All I'm trying to do here is knock up a piece of metal with 5 irregular spaced holes in it. Fusion is fighting me all the way. Do I draw the metal boundary then on different sketches have five circles or all as one unit? if I miss a hole and have to add it is this a new sketch or find the original shape and edit that? I cant force a snap to an intersection, the copy has disappeared from the Move/Copy command why cant I have a symmetrical array (sorry pattern), is the term chain is this the same as a Pline. I have tried to insert a MidPlane on a bolt head but use the pointy bits not the flats - no there is no option to choose a line, it has to be a face - why? the software is just not intuitive to use which is a great shame. 

So what you see here is the result of many many hours work - I really want to learn F360 but the chaps and chapesses over at Autodesk are making it SO hard to do so.

Anyway  I've my moan for the evening 

Thank you again for you help - I think Dm is the way forward for me 

Matt

[Phil.E]

Here are some answers to your questions.

The reference of the canvas doesn't disappear. It simply cannot be shown because it hasn't happened yet at the point you are rolling back the timeline by editing the sketch.

To edit a sketch without rolling back time:

1. Make the sketch visible

2. Right click on it in the browser, and pick Show Dimensions.

3. Edit without rolling back time.

I would recommend 100% verb noun workflow for you. The command dialogs do a great job of filtering the available inputs with no ambiguity.

If you want to do noun verb workflows, use the Browser to make selections if at all possible, such as body or component selections, again, no ambiguity selecting the correct object.

Have you looked at the Learning Page?

• http://help.autodesk.com/view/fusion360/ENU/

In every section there is a hands on guided tutorial. Just click into the sub heading pages to find them.

The files required to actually do the tutorials are already uploaded in your projects as "Basic Training".

There is one more level of instruction, a little deeper. It's called the Adoption Portal.

• http://f360ap.autodesk.com/courses
• There are over 100 guided tutorials there.

You can also enjoy all the free content at Autodesk University. You can watch the video and download the white-paper.

70 Fusion 360 Tips in 60 Minutes

https://help.autodesk.com/view/fusion360/ENU/courses/AP-2019-60-FUSION-360-TIPS-IN-60-MINUTES

Fusion 101

http://au.autodesk.com/au-online/classes-on-demand/class-catalog/classes/year-2016/fusion-360/pd1815...

Master assemblies class

http://au.autodesk.com/au-online/classes-on-demand/class-catalog/classes/year-2017/fusion-360/lo-dm0...

Regarding command prompts, you might have turned that off in preferences. Each command, at every step, Fusion should be trying to help you with command prompts. Please let me know if you find a command that doesn't have an accurate prompt when needed. I can log a bug and get it looked at.

Regarding the workflow questions:

• Once you have the reference Canvas on screen, you could make this part a number of ways.
• If I was using AutoCAD to make the part, I would draw the bean shape and holes all as one sketch and extrude it in one operation. You can do that in Fusion too.
• If you miss a hole, edit the sketch that should contain the missing hole, and add it.
• I have no idea why you can't snap to an intersection, it works well inside Sketch. Please show an example so I can understand why it fails for you.
• Circular pattern symmetric is an option, look in the dialog, on the dropdown menu for Type.

• Chain does not mean Pline, but I see what you are saying. Chain is any set of connected edges or sketch lines that the command using "chain" can consume.
• For your bolt plane, try Plane at Angle, use the center line of the bolt, and add your angle. 60°. No face selection required.

 Here is a video showing how I'd make the part you are trying to make. Late in the video I undo several sketch circles and use circular pattern instead.

 Good luck, let me know if I can help more.

Regards,

[drewmerrill14]

I found this really helpful, This always happens and I'll I need to do is move my canvas before my sketch in the timeline, perfect! Thanks!