Extrude and share sketch problems.

[Squawk]

Hello,

I've been breaking my brain over this..

Somehow I can't extrude several shapes in my sketch. I can't see the "share sketch" option in sketch 1.

After extruding 3 things, there is no extrude part available anymore, even though sketch 2 could be set to "share sketch".

I really need help with the following:

- why can't I choose "share sketch" for sketch 1?

- why does the "share sketch" feature of sketch 2 not allow me more than 2 extrudes?

- I made 2 sketches so that when I would use extrude, I can select an extrude per sketch. However, even though I select sketch 1, when trying to extrude sketch 1, it allows me to select sketch 2 features as well. Why?

- I cannot slelect the the feature without the round circle with legs, only the whole thing or the round circle with legs (see pictures). Why?

I hope somebody will have the time and energy to help me out..

Thanks in advance!

Squawk

[Squawk]

JD, if I may ask..

As you can see from the attached picture, I've already put your help to the task! 🙂

I used the case picture and made it to the size of the inner dimensions measured close to the corners.

Only thing is, as you can see, the case is both a bit "curved" on all sides and there is about 5 mm difference between the dimensions measured close to the corners and in the middle of each side. And also, the case is a bit tapered.

Now when extruding this, I can choose to taper it. But the effect is somewhat strange when also having "curved" sides and those 2 parts sticking out at the bottom of the drawing (the 49 - 67 x 24 parts).

Since the foam inlay is kind of hard, I should really make it the correct size.

Is there any good approach to getting the inside of this case drawn in Inventor to accurately reflect a solid block of foam?

[JDMather]

I can't tell, but it doesn't look like you have the image the correct size.

Sketch a line across the image between two easy to measure points on the real part.

Dimension this line.

Chances are the dimension of the line doesn't match the measured points on the real part. 

Add a horizontal constraint to the image frame.

Dimension the image frame.

Double click on this dimension and whatever the current value is multiply by (real part size/dimensioned line size).

This will scale your image to 1:1 relative to the actual part.

I like to then manually center the image about the origin and then add a horizontal and vertical constraint between the origin and the image frame to lock it down tight. Finish sketch and then start new sketches to create your part geometry.

Send me an email for the tutorial files.

[Squawk]

Thank you for your help JD!

On the picture it is hard to see, but the case has a "ridge" inside. The inner dimensions from this ridge are what I made in Inventor.

It is correct that the image should be rotated -0.15 degrees to be "horizontal". Did that the way you sugested and added the horizontal constraint.

The reason you want the center of the case to be the origin point is to facilitate patterned sketches (symmetry)?

My e-mail address for the tutorial files is: kpublic@ziggo.nl.

Thank you for wanting to send them to me! Much obliged.. 🙂

[JDMather]

You should not post your email here.

Email me directly and I will reply with the files attachment.

[Squawk]

I can't edit my post anymore..

Will e-mail you directly.

One more question..

Is there a way to cut off the extruded part in such way that the outer surface of the extruded part tapers to the blue line dimensions in this picture?

(The yellow dotted line is the original sketch surface, the solid yellow line the outer part of the extrusion and the blue solid line where I would have wanted it to taper to..) (Attachment holds larger better visible picture.)

[JDMather]

Edit the Extrude feature and on the second tab set the Draft angle.

There is a chance this might not give the results you expect.

In that case, delete the Extrude and instead Loft from the base sketch to the blue visible sketch.  (you might first change the yellow projected lines to construction so that the Loft doesn't select those)

[Squawk]

Yess.. 

It got the desired results using "loft".

This would have taken me days to figure out without your help!

Thank you so much for spending your time on me!

[Curtis_Waguespack]

Hi Squawk,

You might give this link a read, and consider it as you go forward in your Inventor adventures:

http://inventortrenches.blogspot.com/2011/03/inventor-101-simple-fully-constrained.html

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Squawk]

Thank you Curtis!

I can recognize the noob in me just looking at that first picture.. lol

Will go through them for practise!

[Squawk]

I had to change some values on the original sketch to get the shape right, but the loft didn't change along with it..

So I decided to do the loft steps again from a previously saved step.

And I can't get it to work anymore..

I needed a work plane to project the geometry on from the original sketch and then loft it to that new geometry on that new work plane.

Just like the first time, I couldn't create a parallel work plane, so I extruded the original sketch as much as I wanted to loft it (170 mm) and then create a work plane on the outer surface of the extrusion. Then project the geometry on that work plane. Then delete the extrusion, but keep its sketch dependencies and all.

Only this time, only 3 lines stayed yellow, the rest stayed pink. (Meaning not contrained/dimensioned?)

Needless to say, the loft didn't work and reported several errors.

No matter what I did, I could not get it to work again like the first time.

So after a hour of desperate attempts to get it right, I decided to restart from scratch. Then as in JD's and Curtis's Inventor help tutorials I tried creating the case around the center point this time.

The initial rectanble was blue, contrained and dimensioned around the center point.

But as soon as I tried to make the two shapes on the bottom and it was no longer a rectangle, I could not get it to turn blue again.

Auto contraint didn't report any "open" dimensions or constraints and the sketch dokter didn't report any problems either..

Just when I thought I got it...

I'm getting desperate here..

[Squawk]

Why can't I get this sketch to turn blue (constrained and dimensioned)?

[Squawk]

Ok, an update..

I had to change some values on the original sketch to get the shape right, but the loft didn't change along with it..

So I decided to do the loft steps again from a previously saved step.

And I can't get it to work anymore..

I found out the "Loft" step didn't work because the original sketch had issues (kept green: not constrained/dimensioned).

The weird thing is that auto constraint didn't show any missing. I use this feature to check, as wel as checking the sketch with sketchdoctor.

After I removed a few dimensions, the auto sketch offered 2 items. I clicked it and found that it was that strange "arc through 3 points" origin that needed dimensioning. What was weird is that it didn't show this before I removed some dimensions.

Either way, I undid the auto constraint thing and entered the needed values myself.

After this, I could continue.

I needed a work plane to project the geometry on from the original sketch and then loft it to that new geometry on that new work plane.

Just like the first time, I couldn't create a parallel work plane, so I extruded the original sketch as much as I wanted to loft it (170 mm) and then create a work plane on the outer surface of the extrusion. Then project the geometry on that work plane. Then delete the extrusion, but keep its sketch dependencies and all.

I found that if I removed the extrusion (keeping the work plane) and then did the projected geometry, there were no problems and I could finish it.

There are however 3 things that I stumbled into during this ordeal:

1.

How can I create a parallel plane to the XY plane (in this case 170mm below the XY plane) without "cheating" my way around this via an extrusion that I later on have to delete?

2.

How is it possible that the auto constraint and the sketch doctor don't show any problems/unfinished features, but yet the sketch remains green (undimensioned/unconstrained)?

3.

Why does the rectanble that I originally made (480 x 383) and centered around the center point loose it's blue (dimensioned/constrained) status after I alter the bottom line in the sketch with some profile?

I appreciate any help. 

I hope you guys ain't fed up with me yet..

[Curtis_Waguespack]

Hi Squawk,

1. How can I create a parallel plane to the XY plane (in this case 170mm below the XY plane) without "cheating" my way around this via an extrusion that I later on have to delete?

• Select the XY plane and drag the new work plane down using the distance arrow manipulator. The Offset value input box displays with a numeric value in it as you drag (if not, clear all selections and then try again).
• Enter 170 mm in the Offset value input box to specify the exact distance from the XY plane.
• Click the green check mark to create the offset plane.

2. How is it possible that the auto constraint and the sketch doctor don't show any problems/unfinished features, but yet the sketch remains green (undimensioned/unconstrained)?

You might have had some relic geometry in your sketch. This happens when we delete lines, etc. and a constrained endpoint or something similar gets left behind. Keeping your sketches simple to start with will resolve having these types of issues in most cases.

3. Why does the rectanble that I originally made (480 x 383) and centered around the center point loose it's blue (dimensioned/constrained) status after I alter the bottom line in the sketch with some profile?

It sounds like a parallel sketch constraint was inferred when the rectangle was created, and then removed when you altered the bottom line. Or something like that, anyway. 

When you're trouble shooting sketch geometry it's often helpful to show the degrees of freedom, and show the constraint gyphs.:

Show or hide Degrees of Freedom glyphs

http://help.autodesk.com/view/INVNTOR/2014/ENU/?guid=GUID-A5B9F70F-763C-47F0-99F7-334ABEE3AF19

Control visibility of constraints

http://help.autodesk.com/view/INVNTOR/2014/ENU/?guid=GUID-99AF5EFD-D0BD-4317-A9C8-E63C3725E83A

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Squawk]

Thank you for your reply and help Curtis!

Ok, I found out why I couldn't get the workplane working.. (no pun intended).

It was so huge that I didn't see it.. only a haze over my drawing..

It was about 15 times larger than my drawing itself and I had to zoom out a lot to see its full dimension.

Of course I could make it smaller and fit my drawing better, but is there a way to make it smaller by default?

Well since there is even a name for it ("relic geometry") it probably means I'm not the only one noobing myself into that problem.. 😉

If I can ask, how would you sketch this simple figure (.ipt file attached) ?

I got problems when I removed the dotted construction lines. I didn't want to see them in my .dwg drawing, and I thought since I dimensioned the arc values it didn't need the dimension from the construction line anymore..

The way I build it up was:

1. draw construction lines left, top and right

2. draw the shapes on the bottom

3. draw a construction line between the two shapes

4. make a construction point in the middle of each sides and dimension it my desired value from the construction line

5. use the arc feature and run the arc through the corner points and the construction points ceated above.

6. dimension the arcs.

Would you do it differently / is there a better way?

And would you just leave the construction lines or also remove it?

[Curtis_Waguespack]

Hi Squawk,

I haven't really been following this thread, so I've likely missed some of the particulars, but here is a real quick rendition of the box with a foam insert.

The important part of the simple sketch approach is to create multiple, easy to create, and easy to modify features.

Have a look at the attached part and use the red End of Part marker in the feature tree to roll back the features. If you roll back all of the features and step through the model one feature at a time, you can study the way this model was created. Others Inventor users, would likely have done some things differently than I have, but most would abide by the simple sketch rule of thumb.

As for your question about the construction lines: Don't worry about extra lines in your model. When you make your detailed drawing, none of the sketch stuff will show up, so you don't need to trim or delete "extra" lines like you might have if you've used AutoCAD in the past. In fact you typically do not want to trim or delete lines in your Inventor sketches because when you do it removes some of the sketch constraints that were holding your sketch together.

Post back if you have more questions, and I'm certain someone will offer some suggestions. Most of us went through the same struggles when we started out, so hang in there.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[JDMather]

Somewhere in all of this discussion you have missed the point (pun intended) about using the Origin center point for symmetry.

You have still placed the origin at a corner even though there is obvious symmetry available in the design.

Use Equal (=) constraints, (or symmetry constraints) rather than duplicating dimensions.

[Squawk]

Hello Curtis,

Thanks for your time helping me out!

I opened your file and rolled back the actions to get to this drawing.

Also I started to try to draw the same steps.

But I can't see how you created the "sketch 2 and 3" and why it says "projected loop" at sketch 2.

You didn't use "arc - three point" there, so what was it?

Google searches did not bring an answer on "projected loop".

I haven't had any AutoCAD experience (unfortunately), my wish to clean up those lines was to make my already busy sketch less busy..

I'm going to wait for answers on this first, before dissecting your drawing more, or I'll be lost.

By the way, I started reading through some of the tips, solutions and info you have on your "From the trenches" website.

Your way of explaining is quite noob friendly and the jokes are hilarious.. Kind of soothes the agony of learning all this stuff.. 😉

And yes, I have a really big stapler here, but fortunatly no co-workers.. lol

Ps. Please never reveal to me how long it took you to make to make that foam example file for me..

[Squawk]

Thanks JD for your patience!

At first I lost my constraints after centering the initial rectangle around the center point.

But since Curtis advised me not to remove any (construction) lines needed to initially dimension stuff, I didn't have that problem.

This is now how I tried to rebuild the part folowing the steps from Curtis's file and my dimensions.

Since you mentioned its better to use the 'equal' or 'symmetry' constraints and added that picture, I was wondering if you meant they could already be applied to the green line here above in this foto, or if you were referring to dimensions further down the construction of part?

[JDMather]

A Projected Loop is created by selecting a face (rather than an edge) and selecting Project Geometry.

[JDMather]

With your new sketch

create a vertical construction line from the origin to the midpoint of the horzontal line.  You can then use this to add a symmetry constraint to the two angled lines.

Select the symmetry constraint

select one angled line, then the other, then the line of symmetry.