How do you modify a sketch that has already been dimensioned?

[JonSchaeffer]

I have a an assembly that I have been working on for quite a few weeks now.

I have realized an issue with starting and stopping on a project like this is... I didn't keep track of exactly where I left off.

And now that I am modeling other components to build the assembly I have some threaded holes that are not in the right place and some countersink holes in a new component are not lining up with the threaded holes I made a while back ago. When I try and re demension them it tells me it is over constrained.

I havent the foggiest idea how to fix the original threaded holes to the right location.

Can anyone help me with this?

By the way when I pull up the sketch it does not show the demensions that are over constraining the sketch when I try and fix it.

I thought just deleting the demension would do it but I can't see any demensions.

[jeff_strater]

I'd be happy to help. Can you attach the file, or share it with me at jeff.strater@autodesk.com?

Jeff Strater (Fusion development)

[JonSchaeffer]

Ok I gave you an invite and sent a screen shot on what I need to do. Let me know if this is clear what I am trying to do...
Thanks!

[jeff_strater · Accepted solution]

Jon was kind enough to share his model, and let me post the results, in case others can benefit.

I was able to modify these holes.  Doing so revealed a few workflow weaknesses in Fusion

First, I had to find which sketch to modify!

Even before that, I had to turn off some components, to be able to see the holes:

Then, I needed to find out what feature those holes were.  I used Select Other (hold down the left mouse button for a second, the Select Other UI will come up, and click on the "Parents" tab):

Select the Extrude feature.  This is now highlighted in the timeline.  Oddly, this feature has warnings, but I don't think they relate to the sketch at all:

Then, I had to edit the feature to find the sketch.  This is one thing that I think needs to be fixed.  We should have an "Edit Sketch" item on a feature.  Instead, you have to edit the feature, and use the same browser trick to find the sketch:

so, now I know that Sketch34 is the one I am interested in.  But, unfortunately (this is another thing that needs to be changed), you have to first turn on the visibility of the sketch folder:

now, finally, we can edit the sketch.  This is pretty straightforward.  I added a vertical construction line between these circles, to keep them aligned:

Then, just add a dimension between the construction line and the right side:

and exit the sketch.  The holes are now repositioned:

Finally, the warnings on this extrude bother me.  I think that's a bug.  But, to fix it, I just changed the type of the extrude to "distance":

I apologize for the length of the response, and if any of it is overly obvious.

The 3 items I was able to distill from this exercise:

1. there is a bug with that Extrude - I'm not sure why it is showing warnings.

2. Fusion needs a way to select a feature and edit the sketch for it, without having to search around for that sketch manually

3. Edit sketch already makes the sketch you are editing visible, but does not check that the sketch container is visible.  In this case, I was able to edit the sketch, but did not see anything, because the folder was set to "off".

There are probably more...

Jeff

[JonSchaeffer]

Jeff thanks for leaving the original model for me to do this myself.
I was hoping you were not just going to fix it for me.
It worked great.
-Jon

[TrippyLighting]

One workflow mistake that I've seen over and over again is that senible naming on different elements is missing.
If one simply keeps the system provided names in place, such as Sketch 1 Sketch 2, Joint Origin 1, Joint Orign 2 etc. then it is no surprise whatsoever that things turn sour once you have to troubleshoot a problem.

So one habit that definitely helps speeding things up is "Providing  sensible naming to everything" to help yourself in navigating your data.

[JonSchaeffer]

So you name your sketches too?
That kinda seemed like twice the work to me. I will give it a try.

One thing I did find was, once the components list became fairly large it was time consuming just reading the list looking for the one I was looking for. I found scrolling my pointer over the list quickly showed me what I was looking for, by highlighting the component it fell on.

[Anonymous]

Lol. Want to know how to move that hole in SolidEdge? Click on it, grab the steering wheel, punch in the distance change, and hit return. Good lord.

[JonSchaeffer]

So quick to lash out with sarcasm and charge someone with ignorance without an ounce of useful help Lukepighetti. There are tons of great softwares out there and they all have great features some better than others, some not so good. Remember this software is in it's early stages and has a community available to make suggestions. Please don't clutter the forum community with these type of comments. If this was an easy task we would all just develop our own software to work the way we want it, wouldn't we?

And I apologize for me calling you out on this as well. I can see you have a weakness for what seems so simple and logical, I have a weakness for sarcasm.
I honestly hoped just like you that I could double click on the feature and an edit button would appear with all it's linked items and I could text in what needed to be finished on my model. So please put your ideas in the "Fusion 360 IdeaStation: Request a Feature or Enhancement of the forum" so people can "Like" it and vote how they want this software to be like...

[Anonymous]

Sorry! You are correct. I have to remember that every piece of software is different and there are DEFINITELY things that Fusion does that Solid Edge couldn't dream of doing... thus why I am using Fusion!

I take your comment very seriously and I am glad that you have said something. I hope I can improve my attitude on here as everyone is very helpful and I certainly don't want to be "that guy."

I will say that an "edit sketch" feature would be excellent! I do like the history bar *A LOT* but sometimes things get so far back on the list it's hard to dig it out when you need it.

Again, thank you for the reality check and enjoy the rest of your holidays.

[TrippyLighting]

Well, if one has created more screen casts to explain things that are not working and reported 9 bugs of which three repeatedly crashed Fusion 360 and one of them lead to a hot fix does that not qualify for at least a little sarcasm ?

I must say I've been biting my tongue 😉

But honestly, I've spent $300 to be granted the priviledge to help in early beta testing. Ahh..sorry..not bitten my tongue hard enough!

IN general though, it is a compliment that F360 is so often compared to Monster Tools (in terms of abilities and price) such as Solid Works, Solid Edge etc.

IIRC the base license for SW is easily $5000 and you'd have to add $2500 for the mainenance subscription to be eligible for updates. 

[TrippyLighting]

Make that report for bug #10 & #11. I thought that there must be an easier way to create a rectanguar hole pattern and edit it. Ant it may, if the hole tols would work as expected.

[JonSchaeffer]

TrippyLighting, I asked for someone to help me. And through the process of figuring out my issue, there were multiple issues caught and honestly admitted to. I'll take that kind honesty and vulnerability over a cover up and the possibility of no help. I see accountability with this as well. They are holding each person involved accountable to all issues, so this has the formula for success. Nothing is being hidden, and for that I don't feel ripped off. Yeah I get frustrated with the glitchy issues. and yes you are right we spent money to be the testing of the software. But Ive never seen sarcasm ever work in a productive way. And probably the majority of people will thrive on the moment to say something sarcastic. I am hoping maybe saying something about it will challenge others to step up their game and focus the energy towards making your software a world class leader in this over priced market.

[TrippyLighting]

JonBoy,

I fully agree and that's why I have tried to avoid sarcasm. Never mind my not quite so serious post earlier.
I will certainly continue with Fusion 360 as its really fun to work with and on the Mac platform there is not competition. so there's a big Kudos for Autodesk for taking that on! Rome was not built in one day either 😉