Fraction Issues
Can you export the f3d file and attach. Never a good idea to leave a sketch with no dimensions, is there still a problem if you fully constrain the sketch?
Thanks Mark
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Just noticed in your screencast at the 4 minute mark you drag the centre point of one of the arcs and you drag it down as well as to the left, if you'd added dimensions to the virtual lines this wouldn't happen. Also you should add a constraint between the vertical line and the circle centre to make sure it at the quad point.
Edit The drag down might be just an visual illusion as the input box moves, not sure. I don't work in fractions but just testing it looks like as you drag everything under 1/64 is fuzzy. Move doesn't snap to the grid so as soon as you drag something it's position is somewhere around +/- 1/64. If you just drag the centre point by just grabbing it with the mouse pointer it will snap to the grid by the way.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
@Anonymous: This is on my to-do list, just haven't gotten to it yet. My theory is that it has to do with dragging/snapping with fractional units. In general, dragging is not precise. Snapping can allow you to snap to certain values. However, if you want precise distances, the only real way to assure that is to type in values, or use dimensions.
Jeff
Jeff Strater
Engineering Director
OK just tested a bit more with fractions and drawing anything just by dragging to a size and not entering a dimension is just fuzzy, +/- 1/64. The lines don't increase in 1/64 steps as the dimension shows. Draw a line and dimension it then draw a line next to it and just drag it's length and you see the problem.
See the line being drawn show 1/64 even though it's half the length of the dimensioned line! You could set a fixed grid of 1/64 but you'd still need to make sure you're at a snap point when you click.
You'll see the same problem working in other units as well especially if you use a coarse precision, here an example in mm.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
The golden rule with sketches in solid modelers like fusion is, Fully Constrain your sketches. Don't take too much time drawing the sketch just make it roughly the right size and place then press the letter D and add your dimensions. It might seem like extra work but the dimensions are editable and drive the entities they define so any modifications are far easier than in programs with dumb sketches.
You might want to go through some of the tutorials in the help.
http://help.autodesk.com/view/fusion360/ENU/?guid=GUID-962B7698-D862-4D7D-AB33-EEE39542DD2F
Here's a screencast with your file, you'll see that when dimensions are added there's no errors. With the dimensions added you have the option of changing a dimension to driven so you can drag then change back to driving to get the accuracy you want.
Mark.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
There's an old expression, Use the right tool for the job. If you want to bang in nails use a hammer not a screwdriver. There are overheads using a history based solid modeler, if it's not worth it for you Fusion's probably not the right tool. I always add all my dimensions so I've not noticed the problem in the 3 years or so I've used Fusion. Don't know if it'll ever work the way you want, the problems been there for years and the forum's not full of complaints because most people follow the rule of fully constraining sketches and with practice it doesn't add that much time. I've used other modelers where there's no history and they work the way you want and yes it can be a bit quicker until you need to edit something, with Fusion it's just a few clicks and it all updates with the dumb modelers it can be start from scratch and hours more work.
Why not add a request on the Ideastation, there might be people who've had the same problem suffering in silence waiting to vote.
Mark
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
I finally got a chance to look at this a bit today. Here is what I experienced: With units set to inch, and with units display set to fractional, I found that, with grid snapping turned on, and the default grid setting of "Adaptive", it seems to work correctly. That is, I can snap to units up to 1/64, and the length is correct. However, if I turn snapping off, then I start to see issues like this. The displayed distance can only go down to 1/64 (Fusion doesn't support fractions like 1/128, 1/256, etc). So, it is certainly possible to have a range of 1/64 of an inch as you drag out the line. It's really no different than if you have decimals displayed, and you limit the precision to two decimal places. What is displayed would be 1.25, even if the length of the line is anywhere betweel 1.245 to 1.254.
Here is a screencast that shows what I found:
Hopefully I am addressing the correct issue, please correct me if I am wrong.
Jeff
Jeff Strater
Engineering Director