A Couple of Feature Suggestions

[Anonymous]

1) When working with sketches, it really should be possible to click on a sketch in the feature tree to select the profiles to be used in a Push/Pull and other operations.

2) When importing models, DXFs, etc., the users default unit selection should be respected.  I have default units set to inch, yet all models are imported with units set to mm.

3) Similar to #2, History should be always ON by default!  Right now, it's sometimes on, sometimes off.

4) When moving sketches, it REALLY should be possible to select the sketch in the feature tree, THEN click Move, then click on a plane or planar model face to move the sketch to.  This would make creating models from 2D drawings (like DXFs) really quick and painless.

Regards,

Ray L.

[TrippyLighting]

A better place for ideas on improvements and feature suggestions is the Idea Station. That stuff gets easily lost in the continuous stream of threads here on the forum.

1. You may want to make a screencast to show how that cannot be done. I can set any sketch in the browser to visible (show) and extrude from existing proiles in that sketch al day long.

3. History is always on for new models. That default can be changed, however in the preferences. The defaulet behavior for importe geometry is always for the timeline to be off, regardless of the preference setings.

4. I am not 100% ure what exactly you mean with "moving" a sketch. However, you can redefine the plane you want the sketch on by right-clicking on the sketch in thebrowser and selecting redefin sketch plane. Then you can select the plane you want for the sketch to be on.

[Anonymous]

1) I think you missed my point.  I wuold like to be able to select the sketch in the tree, then do a Push/Pull, WITHOUT having to select profiles.  It should just use ALL the profiles in the selected sketch.

3) No, it is NOT turned on for imported models or sketches.  Try importing a STEP file, of DXF.

4) There is no Offset Sketch Plane in my right-click menus.  There is an Offset Plane, but it does not change the sketch plane, it simply creates a NEW plane.  The sketch remains right where it was.  Again, this is with imported sketches, which seem to get handled very differently from native Fusion sketches (which is the whole problem...).

Regards,

Ray L.

[TrippyLighting]

1. I did miss your point 😉 That could work, so please put it in the idea station.

2. I did write "The defaulet behavior for imported geometry is always for the timeline to be off, regardless of the preference settings". That means "it is NOT turned on for imported models or sketches" or am I missing something ?

3. You can "Redefine Sketch plane" as shown in the  littel screencast. That works with imported DXF files as well. Again, I am not exactly sure that's what you want to do.

[HughesTooling]

A few comments.

#1 that's OK if you want to use all of the sketch profile\outline but Fusion's not restricted to just the outline.

#2 Yes that has been reported lots of times Fusion reads the units if they're in the file but always opens in mm. If you can use New Design From File it works correctly but you're restricted to igs, stp, sat and f3d.

#3 Personally I want history off for imported models as it makes editing using direct modeling easier, when I have the import fixed up how I want it I turn history on.

#4 With history off you can move and edit sketches see #3, if you've enabled history you'll need to edit the base feature first. There's no redefine sketch plane for imported sketched. If you're working with DXF files have you tried using insert instead of uploading. You can use insert with history on and each layer in the DXF with make a sketch and it has the option to redefine the sketch plane.

Screencast, edit base feature.

Mark

Edit Insert DXF is here just in case you've not seen it.

[Anonymous]

"2. I did write "The defaulet behavior for imported geometry is always for the timeline to be off, regardless of the preference settings". That means "it is NOT turned on for imported models or sketches" or am I missing something ?"

Sorry, I did mis-red your first response.  But my whole point is that should be a global preference setting.  I don't understand the logic behind making it behave differently with different sources.  Its inconsistent and confusing.

"3. You can "Redefine Sketch plane" as shown in the  littel screencast. That works with imported DXF files as well. Again, I am not exactly sure that's what you want to do.

That option is simply not there when the sketch was created by importing.  If I import a DXF file using "Insert", then that option is there, and works.  If I import a DXF using Upload, that option does not show up when I edit the created file.  Why??  There is not a reason in the world for those two operations to behave differently.

This is something that drives me crazy i nFusion.  I find a useful function on a menu, and when I try to use it again later, it's not there.  That happens A LOT.  For example, if I right-click on a sketch, often the Move and Edit options are simply not there!  Or, I watch a video, to learn how to do something, but then find the options used in the video simply do not exist in my software!  I've all but given up watching videos because of this problem.  I don't know if its just due to different versions of the software, something "modal", or something just wrong in my software.  I do know there are seemingly endless nonsensical differences in the handling of Uploaded and imported models and sketches, and those that are created in Fusion.  Clearly there is no techincal reason for this, as, in this case, HOW you get the data into Fusion afffects what it allows you to do with it once it's in there.

Regards,

Ray L.

[Anonymous]

"#1 that's OK if you want to use all of the sketch profile\outline but Fusion's not restricted to just the outline."

I'm not suggesting that be the only option, just an available one.  It is tedious having to manually select all the profiles in a sketch when you want them ALL.  Clicking on the sketch in the tree is an obvious shortcut.

"#2 Yes that has been reported lots of times Fusion reads the units if they're in the file but always opens in mm. If you can use New Design From File it works correctly but you're restricted to igs, stp, sat and f3d."

But why the inconsistency?  It makes no sense, and rather seems like someone was too lazy to add the few lines of code to make it work right.

"#3 Personally I want history off for imported models as it makes editing using direct modeling easier, when I have the import fixed up how I want it I turn history on."

Again, the issue is consistency.  If you want it off, you can always turn it off, but the behavior should be consistent, and NOT depend on the file type you imported.

"#4 With history off you can move and edit sketches see #3, if you've enabled history you'll need to edit the base feature first. There's no redefine sketch plane for imported sketched. If you're working with DXF files have you tried using insert instead of uploading. You can use insert with history on and each layer in the DXF with make a sketch and it has the option to redefine the sketch plane."

See my previous response.  What you can do with a sketch is very much a function of HOW that sketch was created.  When you a) create a sketch in Fusion, or b) Upload a DXF, or c) Imsert a DXF, you get DIFFERENT results, and some operations, like changing the sketch plane, disappear.  It makes no sense.  I have encountered MANY such issues with imported and uploaded geometry from DXFs and Solidworks files, rendering the import capability in many cases nearly useless to me.

Regards,

Ray L.

[HughesTooling]

There is a difference between insert DXF and importing through the date panel. Insert will only import 2d info, import will import 3d sketches, I suppose if a sketch is flat\parallel to one of the construction planes a sketch plane could automatically be created but there could be times it woldn't work. Perhaps they decided to make it consistent and not create sketch planes for imports.

Mark

[Anonymous]

Mark,

Both will create individual sketches for each layer, the only difference
being that when you use Upload, all those sketches are placed on the same
plane, and you do not have the option of moving them using Redefine Sketch
Plane. You CAN move them using Move, but it is neither easy, nor
intuitive. For 2D DXFs, both approaches should behave the same.

Regards,
Ray L.
jagboy2013@gmail.com
(831) 234-0858

[Anonymous]

And.....  I'm stumped once again.  I import the DXF using Insert, which gives me all the layers in separate sketches.  What I want to do is use those sketches to construct a 3D model.  So, I Pull one layer to create a solid body.  Now I want to Redefine Sketch Plane to put another sketch on one of the faces of that body, but I CAN'T!  The sketch I need to move appears ABOVE the one I've already Pulled in the tree view, so as soon as I click Redefine Sketch Plane, the body disappears.  It appears to be impossible to re-order the sketches in the tree view, to put them in the correct order to allow me to do what I want.

Is there a way to do this, short of manually moving all the sketches using typed-in offsets (which will create a very "brittle" model)?

I will also want to "connect" sketch entities in one layer with features created by extrusion from other layers.  For example, one payer may contain a counter-bore for a hole created in a lowere layer.  I want to force that counterbore to be concentric to the hole, so if the hole is moved, the counterbore follows it.  Is that possible?  This is all very easy to do in Solidworks.

I'm starting to believe importing anythig into Fusion is nearly useless if you want to modify the imported geometry in any meaningful way...

Regards,

Ray L.

[HughesTooling]

After you import a file with layers the sketches are grouped, right click the group in the time line and select delete accept the default option on the next dialog and the sketches will ungroup. Now you should be able to drag the sketch along the timeline past the extrusion and redefine.

Mark

[HughesTooling]

Just in case my ramblings didn't make sense here's a screencast.

Mark

[Anonymous]

That works, but not quite the way you described.  First Delete to un-group (sketches that are not obviously grouped) is waaaaaay counter-intuitive.  There is no way logic and reason would lead me to try Delete in that circumstance.  But, it did un-group the sketches.  Once un-grouped, I can re-order the sketches in the timeline, but that changes nothing in the tree view, which also seems counter-intuitive to me.  I can live with that.  

But, once I create the first body, I can no longer re-order sketches EXCEPT within the list of sketches.  I cannot move any sketch PAST that first body as you suggested., nor can I move the body back INTO the list of sketches.  What I had to do was first, order the sketches as I wanted, then roll-back the time-line to the first sketch, Pull it to create the first body, then roll forward to the next one, Pull it, lather rinse, repeat.

Why am I not allowed to re-order outside the list of sketches?  That body should have no dependencies on ANY subsequent sketches, so I should be free to move the other sketches wherever I like.  Also seems to me that will sometimes create problems down the road, once I've created a lot of features, and want to then go back and perhaps re-order some, I will not be allowed to, without first deleting the bodies, then having to re-create them.  Seems odd....

Regards,

Ray L.