How to sketch on the round cylinder surface? need advice (Inventor 2014)

[Sengna]

I was trying to draw the 2 ear pieces with concentric holes sticking out on the round surface. but i am not sure if this is the right way to go, if not any other way? i was using the tangent to surface through edge. i sketched on the horizontal plane but the end of two lines didn't project to touch the surface of the cylinder (Note: see two red arrows). Which plane should i sketch on Vertical or Horizontal? please advice

Roud Hollow Part.ipt

Edited May 19, 2014 by Sengna
details

[Vagulus]

I was about to extend the two sides of the tongue to meet the cylinder when I ran into trouble. Inventor tells me the sides have a dimension and won't allow me to extend them.

 

 

Would someone please tell me why? Thanks

Scaffold_Clamp.ipt

[JD Mather]

In the real world how would that part be made?

All of the white faces are machined faces.

You are trying to violate real world logic.

 

Slotted Part.ipt

Edited May 19, 2014 by JD Mather

[Vagulus]

In the places where I have worked they would take a length of shaft (or thick-wall tube) and two pieces of profile-cut plate and weld them together. Therefore, I saw no anomaly in adding the bit onto the side of the cylinder. I take the point that the central bore should have been done later. However, that was not the problem.

 

 

I was merely figuring out for myself how I would resolve Sengna's issue as I perceived it, and I got into trouble. To solve the matter I had to remove all the constraints and dimensions attached to the tongue-piece. Then Extend would work.

 

 

BTW: Thanks for your IPT file. Lots of good lessons there.

[Sengna]

I was about to extend the two sides of the tongue to meet the cylinder when I ran into trouble. Inventor tells me the sides have a dimension and won't allow me to extend them.

Would someone please tell me why? Thanks

 

I can feel your pain Buddy LOL

[Vagulus]

Hi Sengna

 

 

Did you work through the way JD did this exercise? He simply extruded the tongue right inside the parent block and let the blending take care of itself.

 

 

Run his IPT up and work through his modelling sketch by sketch.

[JD Mather]

In the places where I have worked they would take a length of shaft (or thick-wall tube) and two pieces of profile-cut plate and weld them together. ...

 

Weldment would be 5 parts.

1 cylinder

2 tabs

2 ribs

 

We can do that too.

[ecshclark]

In Sketch 3 use the Project Cut Edge command. This will project the outer diameter onto the Sketch/Workplane. Get rid of that tangent vertical line. Trim the tab edge lines to the diameter. Properly constrain the rest of the geometry. Then Extrude and Cut away as needed.

 

My preference is I would model this as a single part, it would take to much time to do it in 5 parts. Typically, a part like this would be detailed on a single drawing sheet, you wouldn't need 5 drawings. The geometry is simple enough a decent shop wouldn't ask or want 5 separate models and/or drawings to machine and weld this up. If you did they'd think you're half baked. If you have a boss, he'd be concerned why you spent so much time modeling and detailing 5 parts. Oops, my boss is coming , I got to get back to my real work!

[Sengna]

Hi Sengna

 

 

Did you work through the way JD did this exercise? He simply extruded the tongue right inside the parent block and let the blending take care of itself.

 

 

Run his IPT up and work through his modelling sketch by sketch.

Yes Vagulus, that's what i am doing right now, the way he did is very advance but it's good to learn from him. Thanks JD

[Sengna]

In Sketch 3 use the Project Cut Edge command. This will project the outer diameter onto the Sketch/Workplane. Get rid of that tangent vertical line.

Eschclark, how did you get the plane to tangent to the edge of the cylinder? I clicked the tool plane--tangent to surface through edge or through point but i after i select the edge of the geometry nothing happen.

[Sengna]

JD mather, i practiced through your drawing these are the issue that i still couldn't figure it out.

1. on my sketch 6, it said that i have one dim left, i couldn't find what it was?

2. on my Sketch 6, how can i make it show only outer circle (2.5 in Circle) instead of extruded cylinder

3. my 1.5 in dim from center of the half circle (R=.875") to the intersected with surface, the point got moved?

Roud Slotted.ipt

[JD Mather]

Click the Show Degrees of Freedom tool.

It will show where you are missing dimensions (in this case - you are missing a coincident constraint)

 

 

You are also missing a coincident constraint between the point and projected circle - therefore requiring extra dimension(s).

 

I recommend that you go through these

http://www.cadtutor.net/forum/showthread.php?85808-Inventor-101

I will be completing as my time permits.

[Sengna]

Click the Show Degrees of Freedom tool.

.

I did add the one missing dim by coincident via Degree of freedom, good tool to use. However my 1.5 inch dim was moved for some reason, i put the point on the intersection line between the round surface and line( At the red arrow)and it was measured right at the beginning, Is it a big deal? can i still extrude it?

Note: I studied through your thread and will finishing up.

[JD Mather]

Delete the 1.834 dimension and add a Coincident constraint between the point and the circle. Simple!

[Sengna]

Delete the 1.834 dimension and add a Coincident constraint between the point and the circle. Simple!

 

I got it, what does degree of freedom do? i can see that i can move the horizontal line up and down follow the arrow but it am still missing 2 dims.

[JD Mather]

You need to Project Geometry that edge so that you can apply a coincident constraint to tie down that point (Inventor does this for you when used correctly).

 

 

I recommend going through these

http://www.cadtutor.net/forum/showthread.php?85808-Inventor-101

(it's in there)

[ecshclark]

Senga, I did not create or use that plane, it was in the part file you attached. I just ignored it and left it there. It's called workplane2 and it's offset from a workplane1 by 2.5 in. There is no need for these workplanes to create this part, and they are not used in my example/modification of the part. But if you wanted or needed to make a workplane tangent to a cylinder use Plane - Tangent to Surface and Parallel to Plane. Pick the outer cylindrical surface, then pick an origin plane or any other surface or workplane that you want the plane to be parallel too.

[Sengna]

But if you wanted or needed to make a workplane tangent to a cylinder use Plane - Tangent to Surface and Parallel to Plane. Pick the outer cylindrical surface, then pick an origin plane or any other surface or work plane that you want the plane to be parallel too.

Little confuse how to do, when you get a chance please attach screenshot .