Help with 3d sketch

[Anonymous]

I understand there is no 3D sketch mode.  I am used to Geomagic Design where you can change planes within the same sketch.  Below I am trying to join the two sketch pieces with a fillet so the loft has no sharp bends.  I have tried the include 3d geometry command for the points but must be missing something.  Is there a good workflow to create something like this?

 Thanks

[Anonymous]

Hi, one way is to use the sketch fillet tool, but both line segments need to be in the same sketch.  A quick way to accomplish that with what you already have, is in the sketch with one of the lines, use Include 3D geometry tool and click on line in other sketch, which will create purple duplicate line in current sketch.  You can then turn off visibility of other sketch, and do window/box select of everything, right click and choose Break Link, which will turn the purple "projected" line to regular color, after which should be able to select it and other line in same sketch to fillet. 

Another great option is to fillet as much as possible after sketching, using the Modify > Fillet that will then show up in timeline. 

Let us know if you have any other questions.

Jesse

[Anonymous]

Thanks Jesse

Accomplished it with the first method.  Good solution--Ended a lot of frustration!  For something so simple for another program to do, it seems like a lot of work though.  Can you please elaborate on the second method.

[Anonymous]

Cool!  Also you can quickly create 3d lines (i.e. off the sketch plane) in the same sketch by various methods.  For example, if you tilt your view at somewhat of a low angle, then try making a line from a point, should get this triad as shown below, which allows to draw the line in 3D directly:

The method I'm using above is to create reference geometry in the sketch plane to then make 3D vertical lines from, since trying to control angles and dimensions in 3D directly is more difficult.  I then made most of the vertical lines construction geometry and connected their 3D end points.

You can also use the move tool to move existing sketch lines and points off plane. 

Regarding the modeling/feature fillet tool, for various reasons whenever possible it appears better to use this, say for the edges or corners of an extruded object, instead of trying to make the fillets in the sketch (although for your case of making a path for sweep, pipe etc. this doesn't apply).  I don't have the thread off hand, but here is some text from it regarding some reasons to prefer this fillet approach:

"This is a great discussion around best practices in modeling.  I certainly advocate for not putting fillets in sketches whenever possible.  That's not to say "never", for instance if part of the design intent in the sketch requires a fillet then by all means put them in the sketch.  If, however, the filets are only secondary or tertiary level of detail/transitions required for manufacturing, I almost exclusively use fillets as features rather thank sketch entities.  Two reasons:

1.  In the event that you find yourself working with a problematic model, the simpler the feature set that defines the geometry, the easier it will be to diagnose and fix any problems.  Sketches should be distilled down to be as simple as possible, the definition of "simple" is entirely up to the designer or the standards set by a company.  This principle helps reduce the burden of corners <pun> one can paint themselves into in a parametric modeler (this is not unique to Fusion; Inventor, PTC, Solidworks, etc. all can support poor modeling practices that end up with a model that can become riddled with problems and errors).    A very simple illustration of this is say I have a shelled part, the primary shape is built from a  sketch with all the fillet details necessary to create my finished plastic part design.  If that shell fails to meet the requirements of the thckness that you as the user needs to determine "where" that failure is occurring.  Experience tells me that the failure will likely be in the radii of one or more of the fillets.  now I have to edit my sketch to find the problem and the potential for downstream features to be compromised greatly increase and you'll often end up "hacking" the modle to get it to just work so you can move on.

2.  If you are working on somebody elses model and need to "fix" a problem area or add additional detail, say add some reference to a theoretical corner that is filleted, if that geometry exists in the sketch, but not the model, It's pretty easy to make the necessary reference.  If your collaborator adheres to this modeling principle then your job can get done much faster and subsequent users won't be looking at "hacky" models."

I've seen other reasons as well, but don't remember off hand. 

Again post with any other questions!

Jesse

[Anonymous]

BTW, it can be a little tricky getting used to having that triad appear.  You first click to start a line on some point on the sketch, then start moving your cursor upwards, perhaps quite high before the triad should appear.

Jesse

[Anonymous]

Thanks for the detailed info.  I will have to play around with the techniques mentioned.

[Anonymous]

Very quickly made this with the 'triad' method.  I expected to be able to go back & edit the sketch & dimension the lines, but can't add dimensions.  Can't select any curves.

[Anonymous]

Glad to hear you got the triad working well (I found can be tricky to get to appear when starting from sketch plane, seems to be better to start at some point along a sketch line rather than line endpoint). 

There appears to be a trick to enable dimensioning 3d lines.  Once start 3D line (clicked its first point), will have option to directly enter a length value, and then an angle.  Be sure to directly enter a custom length value, and hit enter (3 times I think).  Then you should have the length and angle automatically dimensioned, which can then be clicked on to change the length and angle if desired. 

Interesting stuff!

Jesse

[Anonymous]

BTW I should mention the commentary on preference of feature fillets over sketch fillets is not mine.

[Anonymous]

I found the trick to getting the triad to appear, after tilting the plane, is to get the angle to snap to the 90.0 deg with the dashed line.  I did originally get the straight lines dimensioned as you said, but when I put the fillets in, dimensions disappeared.

**An interesting note: fillets can be deleted & the Extend tool works in 3D!   

Also the method you are using to create the reference points is a work around.  We should be able to enter point coordinates directly, & relative to existing points for this kind of work.  There is a request for direct entry of points currently on the Idea Station.  There is also one for 3D dimensioning.    

IF F360 wants to attract Solidworks & other MCAD users, this functionality has to be there because it is expected.

I am quickly learning the limitations of some features in the software, while being pleasantly surprised by others.  Can't wait to explore more.

[Anonymous]

Hmm, I see that 3D filleting can remove the dimensions.  Well I would probably do something like this like you were originally doing, creating the construction planes such as offset planes, planes at angle. etc, and the sketches on them, connect them with 3D lines in final sketch in which also use Include 3D geometry as we discussed before and do the fillets.  Another option if you want to change a 3D line dimension is to use Inspect > Measure to measure from one relevant point to another, then use Move tool and select all the relevant 3D line and fillet geometry, and enter a move distance based off the measurement that was taken and desired new position.  To change 3D fillet radius like you said can delete the existing and easily create another by clicking on the two relevant 3D lines (interesting observations you made about that and the extend tool). 

Regarding sketching in general, the general approach is to create the desired geometry roughly, before adding exact dimensions and positioning via dimension tool and constraints.  Of course with current limitations of 3D sketching its a little more tricky sometimes 😉

Jesse

[cekuhnen]

@Anonymous Yeah wait till next year then many new toys will be presented to us I think.

I agree some of the tools are lacking details but that will I think be addressed next year.

What I really enjouy about Fusion is how they pack all those tools into a good user interface and workflow!

[derekfriedrichs]

I'm so glad I came across this, I have been struggling with this exact issue, and finally I can sleep again.