Extrude - Command Does not Recognize Sketch Object

[delaing]

I'm following along with a tutorial modeling a board with dovetails.

At the point where Kevin calls the Extrude command and selects the profile to Extrude, in my attempt, Extrude does not seem to see the profile and only sees the face of the already-extruded board.

I created a Screencast showing that if I follow a similar sequence, Extrude will see the square shape/profile and execute the Cut through the board.

In Kevin's, he is building the dovetail geometry in two halves constrained across a construction line.

I have to presume there is still some basic approach to sketch geometry that I don't understand which is preventing me from Extruding. I've followed Kevin Kennedy's steps about four times now and cannot get past this point.

Attached is my tutorial file where the Extrude fails to see(?) the dovetail shape and the square shape(3 lines) at the edge of the board.

I've also had to attach the screencast I made of the simplified apraoch as an mp4 because the usual Upload is not making the video available through this post interface in the My Screencasts dropdown.

What am I not understanding about Sketch geometry or the Extrude command?

Thanks in advance,

Delain

[aliobidi]

Hi , 
1st, your profile should be closed  
2nd, your plane should be the geometry face not a  construct 
3rd , when you done second step the geometry will give you outer sketch then when you do the other 3 line sketches will be closed with the outer edge 

see the "PIC " with new sketch on the geometry face  
your file below 

[jhackney1972]

You dovetail sketch is not a complete profile, you are lacking one side.  Remember, if you have Show Profile on in the sketch dialog box, it will change colors when you pass over it.  If you created this sketch using Symmetry, then you just forgot one line.  See Screencast.

[aliobidi]

plus the line type you used can't make a close profile you should change it to centerline 
see the PIC below 

[delaing]

@aliobidi 

@jhackney1972 

Your information is very helpful and pointed me to the problem, but not sure how it happened. And continues to happen.

The edge of the board profile(?) was solid when I first drew it in the sketch, and then extruded it.

However, when I created a new sketch on its face (to create the dovetail shape) the profile edge inherited the construction line type when I drew a construction line to use it for the Symmetry constraint.

I've created a screencast to demonstrate what happens.

(I cannot get Screencast to list any newly created casts in the Post dropdown list. so I have to download and attach. Very frustrating.)

Now, when I change the profile edge from construction type back to solid, then Extrude will see the square shape as extrudable.

Testing again, if I draw a construction line from the same board edge, it will not convert the edge to construction type a second time.

I attached my test file where you can try this on the bottom edge of the board shape. Draw a construction line off of the bottom board edge. You should see that now that edge will change to a construction type.

Once you convert it from construction type back to solid, it will not inherit a second time, if drawing a new construction life off that edge.

Sorry if my explanation here is confusing. I'm confused as to why this is happening.

Also, note the Constraint-type glyph in my screenshot above.  What is that; what does it indicate?

Thanks in advance,

Delain

[laughingcreek · Accepted solution]

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@delaing wrote:

The edge of the board profile(?) was solid when I first drew it in the sketch, and then extruded it.

However, when I created a new sketch on its face (to create the dovetail shape) the profile edge inherited the construction line type when I drew a construction line to use it for the Symmetry constraint.

I'm going to guess that you have this setting checked in your preferences-

your video you start by toggling on the construction line type.  Then you are selecting the EDGE of the solid. That automatically projects that geometry into your current sketch because of the above setting, and since you have construction line type toggled on, it's setting that projection to a construction line type.  the line type in the first sketch is unaffected.

I personally (along with most experienced users) prefer to explicitly project the items I want instead of having fusion do it for me, so I suggest unchecking that setting, along with the other one indicated in the pic above.

[laughingcreek]

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@delaing wrote:

...(I cannot get Screencast to list any newly created casts in the Post dropdown list. so I have to download and attach. Very frustrating.)

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yeah, that thing's been broken for years.  I can't understand why AD doesn't just remove it and save the confusion if they aren't going to fix it.

you can post a link to the screen cast in the body of your post instead.  the screen cast are nice sometimes b/c they can capture all the commands you enter.

[laughingcreek]

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@delaing wrote:

....Also, note the Constraint-type glyph in my screenshot above.  What is that; what does it indicate?...

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that glyph is the projected geometry constraint.  It can be deleted if you for some reason wanted to un-link it from the geometry it was projected from.

[delaing]

@laughingcreek 

Yes, that first setting was the culprit causing this. I had a hunch it was some sort of setting somewhere.

I had the second setting already disabled.

Still gotta learn about Project and when/how.

Thanks for the other tips. I suppose I can embed the HTML next time for a screencast.

Delain

[delaing]

@laughingcreek 

If I could have another minute or two of your time, could you give me a brief remark on why you do/don't have the highlighted preferences in your lineup.

I want to avoid other traps caused by not having the optimal setup like the original post revealed.

This is my current prefs dialog.

[davebYYPCU]

I will jump in, Preferences are just that, what we can opt in or out of.

For his first and last ones, will leave to Alex, likely the way his workflows, flow.

For me, Auto Look at Sketch is off.  I need a new sketch with 3d camera angle, so that I can see and select my - to be projected articles, easily.

Show ghosted result is off, - clutter.

Hide sketch on feature creation, - off, very rare for me to need that,

as I use sketches for more than one feature, more often than this would help.  

Might help....

[laughingcreek]

I don't use auto hide sketch or auto look at sketch ever.  personal preference.  I want sketches to stay visible, and view point to not  change just because I'm editing a sketch.  for much the same reasons as Dave outlined.

(I've actually seen a lot of questions here that trace back to the the auto hide sketch behavior b/c the user didn't realize that was happening.) 

I haven't used simplify tools yet other than to play around with their functionality, but don't figure it hurts to have more tools available in the tool bar just incase the need arises.

Active component visibility is usually checked (I just happened to have it unchecked when my screen shot above was taken), but I do toggle it off some times. effects visibility of  components that aren't active.  when checked non-active components are translucent, which I normally prefer.

Show ghosted body result is related to T-splines (not sure why description doesn't just say so).  usually unchecked.  When you re-enter t-spline editing, this setting will leave a ghosted (very translucent) view of the brep result body from before entering the t-spline editing space.  suppose to be helpful to use as a visual reference for making small changes.  Mostly just annoying.

[delaing]

@davebYYPCU @laughingcreek 

Thanks to both of you for taking time to explain. I will incorporate and see how they affect behavior.

Delain

[JamieGilchrist]

@delaing,

glad you were able to get it sorted out.  One thing I noticed when you were creating your sketch is using a construction line, I'm sure that was prescriptive from Kevin's tutorial.  Another way you can achieve the same results is by using the Horizontal/Vertical constraint on points.  What I mean is even though a line may be constrained horizontally or vertically, its endpoints or its mid-point (with the H/V constraint active, hold Shift and hover over the middle of the line and you'll see a midpoint snap glyph appear) can be used instead of a construction line in many situations.

In your example, I purposely drew the tree lines "oversized" and then used the H/V constraint tool to constrain the two vertical lines midpoints (this acts in the same way a construction line would).  Added dimensions and it all worked out as expected without having to put any symmetry constraints in place.  Note; you can use the "Shift" hover for dimensions too.  

[delaing]

@JamieGilchrist 

From what I can make out, this seems like a great approach to the same goal.

Is there some way to change the playback resolution on screencasts? It's as if I'm watching the cast through a snow-covered window. I had to review yours twice to see that you had already sketched the lines prior to the start of the recording. From what I've experienced so far, Screencast is very poor.

I appreciate this information. Just earlier today, I stumbled onto a Youtube tutorial talking about this H/V constraint using the Shift-midpoint action.

Delain