Strange outcome after shell command

[Anonymous]

Hi,

I am currently following the 8 video series on YouTube by @TheCADWhisperer creating a scissors jack model.

I am almost at the end of Video 1  creating the base.  I am confident I have followed the instructions accurately up to this point.  I am trying to shell the base as per the video, but getting a very strange outcome.  I've played with the fillet placement trying to overcome the problems encountered in the video, but this is not altering this outcome.

It appears to have shelled out the shape of the 3rd sketch, but I a clueless for the reason this would be happening.

Any help greatly appreciated.

Thanks,

Ryan

[mango.freund]

hello, you stumbled over a mass while switching the command. shell 0.0624in. greetings mango

[mango.freund]

https://youtu.be/YiXJWB0NHxo?t=1258

[TheCADWhisperer]

Do you normally work with inch units or with mm units?

0.625 inch would be a bit thick for sheet metal.

Try 0.0625...

[Anonymous]

Thanks @mango.freund & @TheCADWhisperer,

Exactly the issue. I'm used to mm hence the oversight.

[Anonymous]

Hi again,

Go easy on me.... This is probably ANOTHER schoolboy error.

So, I'm at the end of creating the lifting plate in Video 2 at around 8 minutes in. I'm trying to move the lifting plate outside of the base plate but am unable to do so.  I have tried toggling between the active components in the browser tree, but I'm not getting the same results as in the video. 

After looking through every detail in the videos browser tree to see what is active, and what isn't, I think I may have noticed part of, or maybe the whole problem.

The layout/location of the components, bodies etc in my browser tree are different to the video.  I haven't the faintest clue how they have ended up different.  My only conclusion is I've created the new components in, or from the wrong place, leading to this jumbled order in my browser tree compared to the video.  Would this be stopping me from being able to pick up the lifting plate and move it away from the base plate?  I've got Bodies & Sketches in different positions on the browser tree, and each time I try to select the lifting plate, the model ghosts like a silhouette and when I hover over the body in the model it only highlights each individual face and not the whole body.

If my browser tree order is the issue, how do I go about rearranging it, assuming it is this that is stopping me from picking up the body?

Thanks

Ryan

[davebYYPCU · Accepted solution]

It's not so easy to diagnose without the file.

You made the new component, but set up the sketch and body for the lift plate in the top of the browser.  The lift Plate component is empty. 

Keeping the Timeline Marker at the end of file.  Activate top level.  Same as that picture, 

Open the sketches folder in the top level, and left click drag the sketch into the Lift Body component, the body should follow.  

With that done, don't move anything, use the Slider Joint and then it will stay in alignment.

Might help....

[Anonymous]

That's great, thank you.

Moving the sketch into that component file brought the body/origins over with it, as you said it should.

It leaves wondering where did I go wrong? I created the new component correctly, but from the wrong place??? I think I created it at the top toolbar. As I'm writing this, it is occurring to me that perhaps I should have right clicked over the new component and "create new sketch" from there, instead of create new sketch from the top. Would this be the right approach?

I've moved the part correctly now, and have added the slide function in that position. All works well. However, I still feel something is off... If I activate either component in the browser tree, it ghosts the other component in the model. The video shows the lift plate active at around 9m 30sec, but both bodies/components are solid and in full colour.  I've attached the .f3d to help determine where this is still going wrong.

[davebYYPCU]

For new design files the normal process is to save the file, then you make a component for each real world part of the design.

At the time you make the Component it should be activated by Fusion, and you make that part - then 

make a new Component, it will be activated, and you make your second part.

For some reason you have made the Base without making a component, and when the base was extrude cut you then made that body into a component from the Browser, which leaves all construction before the extrude in the top level.  Live with it, as this one can't be fixed like the second component was.  I can't remember if this is as the tutorial shows.

That said, the file as it is is fine. 

When you activate a component, all other Components are deliberately faded, (still selectable) and the current active component does not fade.  When you activate the top level, all components come back to full colour, so that is expected / normal.

Might help....

[TheCADWhisperer]

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@Anonymous wrote:

1. Moving the sketch into that component file brought the body/origins over with it....

 2. As I'm writing this, it is occurring to me that perhaps I should I still feel something is off... If I activate either component in the browser tree, it ghosts the other component in the model. 

---

1. I don't recall if I mentioned in the video that I created the sketches for the Base at the wrong level in the assembly.

This is a common mistake.

2. You can set the visibility for inactive/active components in Preferences...

[Anonymous]

Thanks guys @davebYYPCU @TheCADWhisperer 

Seems that is the genesis for any design created from multiple components.  Wisdom suggests it becomes my 1st action on any project.

I'm now on video 4 of this series, and have walked into another wall.  With the anomaly surrounding the gear dimensions on the left side of sketch 1, I have tried to follow the steps as instructed, but ended up with a very different outcome.  The 20deg angle of the 2 lines mirrored around the first construction line will not adjust. If I try to delete dimension and re-dimension, inputting 20deg as the required angle, it will not adjust from the 6.2deg it is currently showing no matter what I try.  The sketch is fully constrained now - I had issues with keeping it constrained after the amendment to the circle cut-out on the far right of this sketch in video 3, but that seems to have sorted itself out when I began modifying this sketch.  Is there a constraint in there somewhere that I should look at deleting?

Also, the tangent lines on the far left of the sketch I've drawn intersecting the construction line to the left from the centre origin look off.  I really struggled to place these on video 3, but assumed (perhaps wrongly) that once all of the radii, angles, symmetry constraints etc were defined, that this would replicate the original in the video.  I'm pretty sceptical about my ability to track and trace the cause of this without screwing up the sketch irreparably, and having to start over.

As frustrating as this can be sometimes, the reward one gets from seeing the model come together is a lot of fun, and extremely satisfying. Wish I had given CAD a look years ago, but I guess it's never too late to learn something new!

Thanks

[TheCADWhisperer]

Delete the 6.2°.  

The lines are at the compliment of the direction of the angle that you want.

Drag one of the two lines so that the angle between lines reverses (getting bigger towards the inside of the part rather than smaller).  (Might be sensitive - in my trial using your sketch I just barely moved.)  Then you can add the proper 20° dimension and all is well.

For future reference - when you run into a problem it is probably best to STOP and ask questions rather than digging a deeper hole.

I just tried again to reproduce the fix and I had a harder time than the first time I did it.

It seems to be easier to move if you drag the center point of the R0.25 down.

I had to do it in several small increments.

It should actually be below the horizontal construction line from the Origin.

Now the 20° can be added.

[TheCADWhisperer]

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@Anonymous wrote:

...and having to start over.

I guess it's never too late to learn something new!

I am 64 years old.

I "start over" every year with my students.

I have started over at least 10 times on this particular design. 

(Actually, I practice before I walk into the classroom, so make that at least 20 times I have done this sketch from scratch and I have seen about every mistake a student can make.  But this is the first time I have seen this mistake.  😀 .)

[Anonymous]

Really appreciate your input on this. Thank you.

I'm 44 years old, having to have a serious word with myself about both my short and long term future.  Exploring Fusion 360 has sparked something in me that has some momentum to it.  As far as mistakes and practice go - I don't think a day will pass where I'm not making some kind of a mistake, big or small.  All I can hope for is the wisdom to continue learning from them.

I'm having little success trying to amend those 2 lines. No matter what I try, it continues to revert back to that 6.2deg dimension regardless of me typing in a 20deg value in the pop up box.

I am seriously considering attempting this drawing again.  If I were to start over, how would I go about re-drawing this sketch so as to not compromise the history down the bottom, or other components linked to it, and generating from the correct place in the browser tree.