Anyone else having "unexpected" things happen to solids when adding entities to a previous sketch??

christopher_owens

Hello! Quickly, I created a "main sketch" and extruded a couple of solids from that. Then I went back to the main sketch to add some other entities and the first solids now have voids! OK... modify the solid and add the "new" sketch regions. But when doing a Use and Trim something I am not use to is happening. I quit trying to Trim Extend and just deleted the lines and started over! Didn't SolidWorks have a "Extend to Corner"??? Pick both lines and "Tah-ha" you have a corner! I seem to be getting line segments and extra vertices.

christopher_owens

Plus I get a sketch that says in can't be solved even though all the entities are black and the solid extrudes from it. Odd!

christopher_owens

Here I did a Use edge to create a sketch line. When I Trim it to the arc and line these little circles show up. Those are the vertices of the line used in Use. Never seen those before. AH! I see they have a Use and a Coincident constraint. Guess I don't want to delete these!

lougallo

@christopher_owens This might have to do with what you selected.  If you use the entire sketch we try to select the common body (like a washer example).  However if you select a region and then the region changes with a new void, it will also try to use the common... if possible.  Does that make sense?

jakeramsley

christopher_owens said:

Didn't SolidWorks have a "Extend to Corner"??? Pick both lines and "Tah-ha" you have a corner! I seem to be getting line segments and extra vertices.

You should be able to select to the vertices of both of your lines and make them coincident.  The underlying line in the sketch is infinite, so changing where the end-points are should extend them.  Unless I am getting confused by what you are trying to do.

As for the vertices lying around after trimming; when you trim a line we attempt to keep around geometry that is being referenced/constrained to other parts of the sketch to prevent having to re-make constraints.  As the end-points of the line have coincident and projected constraints to geometry that aren't being removed (the external edge/vertex), we keep them around.

When I am sketching on a face, I tend not to use it and just manually add constraints or points to the edges themselves to get the new geometry that I want.  

christopher_owens

I think I had something like an "L" shaped box. I ended up just wanting a box, so I deleted the "inner L". when I tried to make a corner of what was left using the Trim...I got lost! I was dragging the line to try to meet where the other was... I'll see if I can recreate that!

christopher_owens

Ok..I think I recreated it! In the images Sketch 1 is used to create Extrude 1. Ok, now I want another part driven off the "L Box". So I start by picking the edges/surface , do a USE so I have the L again.   
(I think I extruded a solid then) After a change of mind... I go back into the Sketch and want to delete the "inner L" so I pick the two lines and Delete. Now I want to Extend the other two lines to form a corner. When I do that, I get those little circles! 




 
Now there are two faces in that sketch instead of one even though the lines are "gone"!!



I see now that I was just dragging the line "out into space". Since I have more "experience" now I see I drag the line but hover the mouse over the top line and the trimming will stop there and create a constraint! At first I was trying to Extend then Trim... old habits!!

Also. now that I know to pick the Sketch out of the Feature List (unless you want to Revolve a Surface with a Construction Line Axis!) it will pick all/both the faces, if I pick on the faces I have to manually pick both. When I first did this I got all confused!! (Why is there now a void?? it's one sketch!) I have unlearned!

christopher_owens

I think what I was doing was just a bit more complex with more other surface's "Use" edges. So I ended up with more "lines" then I expected and voids! Plus I started deleting those little circles since I didn't know what they were ("I don't remember placing a Point there? I'll just delete it").

brucebartlett

This is becoming a frustration to me. I constructed a sketch, extruded a solid from a sketch by selecting the sketch then un-selecting the unwanted regions. Part evolved with rad's, shells, etc. Then I decided  at a later point I needed to rotate the part by 4 deg's, I chose to do this from the original sketch but upon rotating, my sketch now intersects other bodies creating a whole new set of regions.

In this case it would be good if I could have just selected the 4 lines I wanted from the construction sketch and had them locked in as the geo to extrude. Not adding and subtracting regions to the extrude command. 

Or a switch to include/not include regions outside sketch in extrude command

What are others thoughts, experience with this?

christopher_owens

@brucebartlett  This is why I "tested" a change to a sketch in a separate file! At least using the "Final" button in the test file only the section had to be regenerated. It is something to get use to and perhaps use to an advantage! I did notice when construction lines cross they don't form regions. At least in a test file I could know what to expect! Sorta...


All I did here was switch the highlighted line from solid to construction and hit "Final"

Another variation of this...


The Sweep is created by the Region defined by the solid circle...
Switching the construction lines to solid...Created these swept Parts!
Seems to depend on how regions are chosen if the Sweep regenerates or fails. Exactly how OS chose to go from one region to four...

christopher_owens

How I got to this you ask?? I wanted to "cut"/Boolean a shape out of a curving surface. So to keep-it-simple I used one circle. Once I got the "complex" Boolean to work I wanted to cut out an angled cut (the triangle shape). Soooo I wondered if I could just modify the "simple" sketch. After trying it in the test file and somewhat figuring out how OS would handle the change (with some "manual" selecting of sketch regions, I got it to work! Somewhere I have images of the Vase I created!

lana

@christopher_owens
Could you please reproduce the multi-body sweep and share the document with support? This looks like a bug to me. Thank you.

3dcad

I've had somewhat good experience on changing sketch behind a bunch of extrusions.. My main problem is constraints, there can be a dozen of icons in one point and it's rather difficult to find correct one to remove to allow certain changes.

andrew_troup

3dcad said:

I've had somewhat good experience on changing sketch behind a bunch of extrusions.. My main problem is constraints, there can be a dozen of icons in one point and it's rather difficult to find correct one to remove to allow certain changes.

Absolutely hear you on the constraint auditing issue.
It's clear that has to get a lot more usable before Onshape is ready for prime time.

christopher_owens

I Shared with Support the above Sweep.

lana

@christopher_owens
Thank you. Actually this is an intended behavior. I've missed the step in your sequence when you edited sweep to reference circular region. The logic we are trying to follow is that patches in sketch are identified by sketch curves bounding them. When topology of patches changes the original reference resolves to patches adjacent to the sketch curves in it.  Does this make sense? If you select sketch from feature list, then we store whole sketch as a reference, which resolves to sketch region. That would have picked up the triangular patch.  Thank you for sharing the document.

christopher_owens

@lana Your Welcome! Being new to Onshape I am just trying things to see how the software "handles" my assumptions! As I learn the workflow of Onshape I know what to expect! And I figure if I post a few of my "trial and errors" it may help someone else!

andrew_troup

lana said:

...The logic we are trying to follow is that patches in sketch are identified by sketch curves bounding them. When topology of patches changes the original reference resolves to patches adjacent to the sketch curves in it.  Does this make sense? If you select sketch from feature list, then we store whole sketch as a reference, which resolves to sketch region....

Could we have Onshape's intentions in respect of a topology change fleshed out a bit more for the general case, perhaps with a couple of illustrative sketch examples of 'before and after'?
I'm struggling a bit to get my head around this topic.

christopher_owens

Here is what I had to get use to in Onshape. For an example I added an Extrude to an existing part. Using the surface of the part as the sketch plane, and a simple sketch with a circle which would be the profile of the extrude. I've learned to select the Sketch from the Feature List instead of picking it in the workspace, because the circle is now three Faces! First time I did this I wasn't expecting that, since I didn't do a Use to include the other entities in the Sketch.



(Selecting Sketch 16 from the Feature Menu)



(Picking within the circle in the workspace)


Again, the first time I did this, I wondered what was happening.

christopher_owens

Now, if I use the surface of the part to Create a Plane (Offset =0) and then use that Plane as the Sketch Plane, sketch the circle, do an Extrude, I can pick within the circle in the workspace, and it is one Face. Sooo, if you want to Sketch on the surface of a part, you can create a "fresh canvas" for your sketch!

brucebartlett

Interesting, I have not noticed that before. This could be  good workaround for layout sketches. Not sure if I will use it but good to know.

traveler_hauptman

I filed this as a bug a long time ago.

If I want to use underlying geometry, I'll "use" it.

If this was intended to be a feature, the UX could be improved. At the very least draw the lines from underlying face in the same line-style as the 'use' lines.

...But it's really a bug for me.

andrew_troup

I think at best it's unduly cryptic, and at worst I agree with traveler-hauptman that it's effectively a bug

ON EDIT: to clarify: I'm talking about the latest example from christopher, where a model edge is treated as though it were part of a sketch if that sketch is created on a face containing that edge. I don't have a huge problem if this behaviour happens only at the time of creating the extrusion, when it will be obvious, but I certainly would have a problem if the circle, later moving across a model edge due to a parameter change, causes that edge to become a silent participant to the sketch.

traveler_hauptman

lana said:

@christopher_owens
Thank you. Actually this is an intended behavior. I've missed the step in your sequence when you edited sweep to reference circular region. The logic we are trying to follow is that patches in sketch are identified by sketch curves bounding them. When topology of patches changes the original reference resolves to patches adjacent to the sketch curves in it.  Does this make sense? If you select sketch from feature list, then we store whole sketch as a reference, which resolves to sketch region. That would have picked up the triangular patch.  Thank you for sharing the document.

@lana It would be super helpful for us if the heuristic for patch selection was documented in the help. Otherwise a lot of us will spend a lot of time like @christopher_owens experimenting to back-out what exactly is going on. I think it's safe to say that engineering CAD users, as a rule, don't like non-deterministic situations. Complex is fine. Magic is problematic.

christopher_owens

I'll add this here since we all seem to be in the conversation!

Just another "what?" creating a feature. I created a Surface (since a Circular Pattern can be created using that and not the Thicken.) So I rolled back the Thicken, created the Circular Pattern of the Surface, and then added the "new" surfaces to the Thicken. Finally I figured out that if you pick on the edge of the Surface the "Surface 11" is added to the Thicken (and then Hide applied), if you pick on the face of the Surface (depending on orientation in the workspace) the "Face of Circular Pattern" is added to the Thicken Feature and the Surface remains displayed. Now the resulting feature is what I wanted, but took a second to catch why the Surfaces were or weren't displayed!

(Selecting Surfaces in the workspace)




(Hidden and displayed Surface)



(Selecting from List with First-Shift-Last)



Better!

Then I tried doing a "Drag-Window" around the Surfaces (with everything else Hidden)



Yikes! Won't do that! I hit the red X before seeing what all that selected!

lana

@andrew_troup , @traveler_hauptman
I'm not ignoring your requests to explain the sketch patch behavior and agree that we'll have to document it. As often happens this discussion made us reassess our thinking on the matter and now we are working on a better solution. Thank you for asking pointed questions.
I'll try to explain the current implementation. Sketch region selection is explained here , I'll talk about individual patches.  If sketch is placed on a face, the edges of this face contribute to creation of patches as well as all the non-construction sketch curves. Each patch is identified by the curves in its boundary with some additional disambiguation data to be able to tell apart regions created by two intersecting circles e.g. . When such a patch is selected as input into a feature its identifying information is recorded. Every time referencing feature is regenerated, its references are resolved by best possible match of identifying information. When additional patches are created or boundaries change, patches adjacent to boundary of original selection are used. This is not easy to reason about and now we see it as the problem it is. Thanks again.

lana

@cristopher_owens This is a window selection issue, I'll file a bug for it, If you report it via feedback mechanism, you'll be notified when it is fixed

andrew_troup

Thanks, lana;  thoughtful consideration is all any user can ask, and it's certainly more than users of other packages generally get.

christopher_owens

@andrew_troup ; @traveler_hauptman ; @lana  Thanks again for all your answers! If you are curious why I am doing so many "what if I do this..." and then asking questions (some of that comes from my experience with the introduction of Pro/E into Caterpillar and training others) I have talked with Onshape about a User Group Meetup here in central Illinois. So I would become the one answering all the "What if...?" questions! Plus I am using Onshape for a GRABCad contest!