Bending a Pipe

[Anonymous]

I wanted to know why it isn't letting me bend these tubes either up or down 90 degrees. 

[TheCADWhisperer]

Exit Sketch1 and Edit Sketch2.

Note in the lower right corner of the screen that Inventor indicates 7 dimensions are needed.

Note the pink points (pink geometry is Inventor's indication of "sick" geometry).

Note the position of the point within the red box in lower right corner of image.

The point is off of the part.

Didn't you notice that you were missing a hole?

Attention to geometric detail is essential in design work.

[TheCADWhisperer]

Now, let's do this right.

Close the file.

Start a new mm sheet metal part.

Start a new sketch on the Front (XY) plane (doesn't really matter what plane, but let's be consistant in following instructions).

Expand the Origin folder and right click on the Center Point and select Visibility.

For now on - you are going to turn on the visibility of Origin and plan out how you will construct your part in relation to this origin.

Look for symmetry. How can you use symmetry.  Use of symmetry might reduce your work by half.  Use symmetry about the origin.

[TheCADWhisperer]

Find the Two Point Center Rectangle tool.

Center implies symmetry.  Hmmmm, that sounds good.  Really good!

Lets sketch a rectangle with the center at the origin.

Note the color of the lines.  (yours might be different than mine - but note the color).

Add the 370 dimension.

Did you see anything happen to the color of the lines?

Add the 120 dimension.

Did you see anything happen to the color of the remaining lines?

Note the "pushpin" glyph on the Sketch1 in the browser - this is one indication that the sketch is fully defined.

Note in the lower right corner Inventor tells you that the sketch is fully constrained.  Checking this is one way to help avoid missing any information that might be needed to make the part.

Exit Sketch1 now.

Save the file with the name Footplate_Rev1.ipt

Attach this new file here for next step (do not try to advance beyond where we left off).

[Anonymous]

Hi cad whisperer I've followed your instruction. You seem to have rightly so pointed all the wrong things on my footplate but didn't comment on the frame it self or the foot frame? What shall I asume about that?

[Anonymous]

390 and 250 are the correct dimensions, I noticed the lines they all went from green to blue and it says fully constrained. Out of interest why does it have to be constrained? and do everything I ever make on Cad have to be constrained? whats the best book to read on inventor to pick up tips and tricks or even the basics?

[TheCADWhisperer]

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@Anonymous wrote:

.... but didn't comment on the frame it self or the foot frame? What shall I assume about that?

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 Don't assume anything.  We will get to that if you don't give up first. (well, you can assume that it is all wrong - unfortunately)

[Anonymous]

I won't give up that easy whats next then?

[TheCADWhisperer]

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@Anonymous wrote:

1. Out of interest why does it have to be constrained?

2. and do everything I ever make on Cad have to be constrained?

3. whats the best book to read on inventor to pick up tips and tricks or even the basics?

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1. Did you see that you had a missing hole?  Fully constraining sketches helps you avoid many simple mistakes.  You send a design like this out to the shop floor with such an error - and it will take months (if ever) to gain back your credibility.  The people on the shop floor will go out of their way to find every error you make and point it out to the boss, rather than check with you first on the inevitable mistakes you will make.  Sweat the details.  This is why you get paid the big money.

2. Yes.  It's my way or the highway.

3. Banach and Jones for beginner, Waguespack (or Munford) for advanced.

[TheCADWhisperer]

OK, as you found you could Extrude this part, but let's go ahead and learn a bit about sheet metal on this simple part.

First thing you need to do is set up your sheet metal Thickness.

Follow this image.

After changing the Thickness, Select Done and then Save Changes.

It should now read the proper value in the box exed out in image above.

Click Cancel to get out of the Sheet Metal Defaults.

[Anonymous]

Well I knew about the missing hole, I shortened it to try and assemble it I was just doing trial and error but now it makes sense the frame itself is wrong, I tried to do my own diagnosis on it I drew the frame again just with the dimensions and without putting any curves on it and bingo the footplate frame and handles fitted perfectly but this could be a fluke.

[TheCADWhisperer]

Instead of Extrude - click the sheet metal tool called Face (it will automatically get your material Thickness).

Flip the direction of the green arrow so that it is going down (I will explain why in next response).

[TheCADWhisperer]

Select the XY plane in the browser and right click start New Sketch on the XY plane.

You could have started the next sketch on the face of the part, but in some cases you could make edits that cause the sketch to go "sick" (remember the pink points).

Whenever possible, use the origin planes for your sketches rather than part faces for the most robust geometry.

This is called the BORN Technique where BORN stands for Base Orphan Reference Node.

You want rock solid geometry that does not fail when editing.  (If you do everything right the first time - you can ignore the BORN Technique.)

[TheCADWhisperer]

Create a 2 Point Rectangle (not center point rectangle) approximately as shown in my image (relative to the Origin Center Point circled in yellow).

Sketch a line from the Origin to the midpoint (you will get a green snap point) of the top horizontal line of the rectangle. (I exaggerated angle to make next step obvious.)

Right click on the angled vertical line and select Construction. (not really necessary, but I wanted you to see how to do this. Then select the Vertical constraint and your angled line should become vertical.

[Anonymous]

This is what my part looks like now note I have the correct dimensions no these are the correct dimensions.

[Anonymous]

Are you sure its on Xy plane and whats the size of that rectangle?

[Anonymous]

my rectangle lines are not visible why is that?

[TheCADWhisperer]

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@Anonymous wrote:

This is what my part looks like now note I have the correct dimensions no these are the correct dimensions.

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 You are not following my instructions - I didn't say anything about adding fillets to the sketch.

In this case - you can leave them there - but it is almost always better to add fillets as features (which I would have showed you) rather than in the sketch.

[TheCADWhisperer]

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@Anonymous wrote:

my rectangle lines are not visible why is that?

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How could I possible answer that question without your file?

The last file you attached did not have a rectangle in Sketch2.

Of course, you have to create the rectangle to have a visible rectangle.

[Anonymous]

Oh sorry yes I've changed my view so now I can see the rectangle.

[TheCADWhisperer]

Dimension the rectangle as shown.

I suspect that since you changed the fillet size that the 100 mm is now incorrect (but I think I will convince you to change that anyhow).

Note that I entered the horizontal distance between holes as a equation ( enter 390-(2*4) Inventor will add the units for you).

Of course with this simple math you could do in your head - but entering as an equation gives it some logic that you might need a year down the road.  And the math isn't always so simple - so let Inventor do it for you.

Technically the 4mm dimension to the edge of the part is a violation of the BORN Technique, but we can consider the manufacturing/inspection datums as well.