How to keep offset constant

[rlkillian]

I'm adding a brace between to vertical members. I always want the offset from the top of the one member to be a certain number, in this case 1", and the offset from the bottom of the other member to be a certain number. Again, in this case 1" but this should be adjustable. I want to do the whole thing as a part not an assembly. I can handle the first offset but the way I did the second one involves computing  the angle of the plane that the diagonal cross section is drawn on (or drawing it in 2d in Autocad to figure it out).  The problem with this, of course, if I change the height of a column or the spacing or anything then I have to recompute the angle and edit it. Not what I would exactly call parametric.

Does anyone now how I could construct this so it would automatically keep the offset at a predefined number? If you look at the attached pdf, I'm talking about holding those two 1" dimensions constant.

[jtylerbc]

I'm still running an older version (2018) of Inventor, so I can't open your file to see how you modeled it.  But I'm not really seeing why you would need an angle to draw this in the first place.  Since I can't see your file, the dimensions in my example (other than your stated 1" offset) are arbitrary.

If you draw the two upright portions first, then you can project their geometry into the sketch for drawing the diagonal.  If drawn that way, you can create dimensions in your sketch that are exactly like what you show in the drawing, and not need to do any external calculations or sketching to get there.

See attached example.

[mdavis22569]

Few ways. 

You could set it up a workplane. Set the workplane. 

Constrain the ipt / 1" to that workplane.

You can also put the 1" in the FX / parameters so it's controlled there as well and assign it. If it does change ...they both can change together or separately ...

I can see a few different ways to go about this .. but was my first thought. 

[Anonymous]

this is how i go about it.

im in inventor 2020 just a forewarning

and now since the sketch is constrained fully, whatever you do to those posts, the middle adjusts with it.

[mdavis22569]

He's in 2018 so it won't open for him 

[jtylerbc]

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@mdavis22569 wrote:

He's in 2018 so it won't open for him 

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I'm actually the one that's in 2018.  The OP is somewhere above that (I couldn't open his file, so I know he's newer than me).  So he may be fine with the 2020 file.

[rlkillian]

@jtylerbc , sorry, I forgot to mention sometimes that diagonal will have a circular cross section. You're idea works great for rectangular cross section. Also, in real life that diagonal would be a tube. Not sure how you would hollow it out. My bad for not explaining more.

But, going with your idea, is there a way to create a construction line at the center of your sketch then use that to create a plane normal to it? The cross-section could then be drawn on that plane then extruded. BTW, what's with not being able to extrude two directions, each to a surface?

Oh cool, I was messing with the model as I was typing this and it occurred to me to try filleting the diagonal. You put in a 4" square so I filleted the four edges with a 2" fillet. It worked! To make it really fancy I linked the extrusion depth and the fillet radius to the width dimension. Now all I have to do change the width in your sketch and it makes a round member. Now all I got to do is figure out how to hollow it out. Oh wait, I didn't realize you can pick both ends with shell to make it a pipe. Playing around with creating another extrusion I found it needs to be a part and not "joined" to properly shell it out. As you can tell I've had no formal education with Inventor.

I would still like to know if the method I mention in the second  paragraph would work but thanks for getting my creative juices flowing.

[rlkillian]

@Anonymous, when I tried changing the post spacing it kinda blew up. Here's a modification of what @jtylerbc did. It makes the square into a circle and hollows it out. You can change it back to a square by suppressing the fillet.

[mdavis22569]

Oops sorry.   

[jtylerbc · Accepted solution]

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@rlkillian wrote:

But, going with your idea, is there a way to create a construction line at the center of your sketch then use that to create a plane normal to it? The cross-section could then be drawn on that plane then extruded. BTW, what's with not being able to extrude two directions, each to a surface?

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This idea would absolutely work, it just requires a little more forethought in the way you set it up.  What you would need is a sketch with construction geometry of the "silhouette", which allows you to locate everything from the offsets as you originally asked. This would then be followed by a second sketch of the profile to be extruded, on a work plane exactly as you described.  If you use this method, the idea would work for pretty much any cross section, provided you set it up correctly with regards to how the two sketches relate to each other. 

When drawn this way, one other advantage is that you can draw the tube initially with a hollow cross section, instead of extruding it solid and shelling it later.  It's good that you learned how to shell the part that way, but with this other method you wouldn't need to do so.

See attached, revised example.  There are certainly other ways you could set this up, but this is one possibility, using Projected Geometry from the Silhouette Sketch to the Profile Sketch to keep the definition of the tube diameter in the two sketches associative.  

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@rlkillian wrote:

BTW, what's with not being able to extrude two directions, each to a surface?

You can, by using the "Between" option on the extrusion.  My updated example file makes use of this method as well.  Doing so prevents the need to make the tube too long and then trim it off in an additional operation.  So I was planning to use it in my example even before I noticed that you had specifically asked about it, just to save myself the extra step.

[rlkillian]

@jtylerbc , that's great! Thanks. I didn't realize you could extrude a profile from something other than the plane it was drawn on. That's cool. I'm learning a lot with this little exercise. I tried recreating what you did but I'm still foggy on snapping. I thought I had snapped the center of the circle to the midpoint of the middle line in the silhouette sketch but Inventor is telling me via "display degrees of freedom" that it's not, even though the circle is riding around with it as I make changes to various things. In other words it seems to be working ok but I've evidently done something wrong. Can you explain what you did to get the center of the circle to snap where you wanted it and the diameter also. I cheated on the diameter and linked it to a dimension in the silhouette sketch. (Can you tell I'm a long time AutoCAD user from my use of "snap"?)

[jtylerbc · Accepted solution]

"Snap" is a correct term to use in Inventor as well.  It just isn't as prevalent as it is in AutoCAD, because constraints replace much of the work done by carefully selecting and using snaps in AutoCAD.  It essentially means the same thing in the two programs, it's just less important in some ways in Inventor.

What I did was:

1. There is a line in the "Silhouette Sketch" that is perpendicular to the tube centerline.  Using "Project Geometry", I projected this line into the profile sketch (Sketch3).
2. When creating the circle for the profile, I snapped the center of the circle to the midpoint of the projected line.  This automatically creates a coincident constraint between the two points.  At that point, the location of the circle is fixed, and it is dependent on the position of that projected line.  At this time, the sketch would say there is 1 degree of freedom remaining (the size of the circle).
3. I added a coincident constraint between the circle (the actual circular curve, not the center point) and one end point of the projected line.  This sets the size of the circle by requiring it to pass through the end of the line, and eliminates the remaining degree of freedom.  The sketch is fully constrained now.

Since I can't see your part (as mentioned earlier, I'm stuck on an older version of Inventor), I'm guessing a little here.  I can think of two fairly obvious things that could be wrong, assuming you otherwise followed my method and just made a mistake.  If you used a different process, obviously there could be issues that I can't foresee.

• If you misclick when doing the first step and don't get the "snap", the automatic constraint won't be created.  This can be fixed by simply manually adding a coincident constraint between the circle center point and the line's midpoint.  This would mean that the circle's position is not defined.  If you are seeing "2 dimensions needed", this is probably the issue.
• If you haven't performed step 3, the position of your circle may  already be correct and tied to the line appropriately, but the size of the circle isn't defined yet.  Add the constraint described in that step, and that should do it.  If you are seeing "1 dimensions needed", this is probably the issue.

Based on how you describe it behaving, I suspect that you have the second case.  

[rlkillian]

John, you've been a big help, thanks. Sometimes I get it in my head how things should work rather than how they do work. I was trying to snap to objects in a different sketch than the one I was working in. Duh. Projecting that line and using that for constraints makes sense.

[johnsonshiue]

Hi Guys,

This can be done in several ways. You can do it with Adaptive in an assembly. Or, it can be done within a part. There should be the first sketch on XY plane dictating the offset and cross member. If it was done in one sketch, it can make things easier. Once you have body geometry, managing the orientation and rotation can be tricky.

Many thanks!