Constraint on points, how to get points, axis

Hello.

I've attached a file of a circular flange that is used to bolt an access hatch to a cylindrical water tank on the curved face. It is a circular ring in flat.

When it's rolled (like it is), to a curvature, there is nothing that is round or cicular. I need to build an assembly with nuts welded to where the holes are to allow bolts to bolt the hatch door to. How do I constrain nuts to the holes? I thought the easiest way is to create some sort of constraint is a work point in the "center" of the holes, but these holes aren't round. I would also then need a work axis through each hole, which requires another work point (one on one side of the hole, another on the other side) so I can insert with the bolt. How can you get these work points?

Any other method?

Thanks for your help.

Regards, David.

Part18.6.zip

Unfortunately (and I just realised this), the development is NOT circular in flat ... I'm not quite sure why, but it's not ...

I'll have to work on this, but my constraint problem still remains nonetheless.

I cant open the file up here at work but are your nuts going to be planar to the flange your bolting to or are they going to just lay on the face? You could create a 2d sketch with location points and project it onto your part. ill try to open it up at home.

Unfortunately (and I just realised this), the development is NOT circular in flat ... I'm not quite sure why, but it's not ...

I'll have to work on this, but my constraint problem still remains nonetheless.

I don't think you want this to be circular in the flat. Although that is often the way the ring will be made because it is cheaper (at least with older manuf processes) allowance would have to be made as it isn't circular when bent.

So the question is how will it be cut when flat - Computer controlled waterjet, plasma or laser (shape will be slightly elliptical in flat - but no problem for the computer) or circular rotating table or tool cut?

If I get time maybe I'll just post either method. I assume the holes will be drilled in the ring while flat. (or will they be cut as above)

In any case I would do one hole and pattern the feature rather than sketch as the patterned feature can be used to automate the placement of the fasteners (pick the pattern and done).

I cant open the file up here at work but are your nuts going to be planar to the flange your bolting to or are they going to just lay on the face? You could create a 2d sketch with location points and project it onto your part. ill try to open it up at home.

Correct, just lay on the face and welded fully around. Can't do 2D sketch as it's rolled ...

I don't think you want this to be circular in the flat. Although that is often the way the ring will be made because it is cheaper (at least with older manuf processes) allowance would have to be made as it isn't circular when bent.

 

So the question is how will it be cut when flat - Computer controlled waterjet, plasma or laser (shape will be slightly elliptical in flat - but no problem for the computer) or circular rotating table or tool cut?

 

If I get time maybe I'll just post either method. I assume the holes will be drilled in the ring while flat. (or will they be cut as above)

 

In any case I would do one hole and pattern the feature rather than sketch as the patterned feature can be used to automate the placement of the fasteners (pick the pattern and done).

Hi. It will be cut circular when flat. The ring, and all the holes - all circular, all cut in flat. When it's rolled, it's result is what it is when rolled from flat. Reason for wanting cicular is there is a direct G-code function for "circle", rather than a series of x and y movements for an ellipse, hence it makes the program much more simple and able to be modified easily by the laser operator in the odd occasion if I make a stuff up Maybe modern software may have a G-code function for ellipse, but our laser and CAM software does not allow.

Correct, just lay on the face and welded fully around. Can't do 2D sketch as it's rolled ...

i understand that its rolled but you can do a 2d sketch off the face and project the points. See attached image. I created a curved face, a 2d sketch with an array of points and projected them to the face.

i understand that its rolled but you can do a 2d sketch off the face and project the points. See attached image. I created a curved face, a 2d sketch with an array of points and projected them to the face.

Hmmm ... interesting idea ... let me have a play with that in the meantime ...

i opened your file up and i dont think that will work out in this case. What i did was create(in your part file) some work axis'. and then i created a plane that was tangent to the surface at a hole in question. You can add two mate to center points of a nut on the axis then constrain the face of the nut to the work plane at that hole. Its a lot of work.

Do you need these in the model for some reason or is this just an exercise. I know you need the part.

i opened your file up and i dont think that will work out in this case. What i did was create(in your part file) some work axis'. and then i created a plane that was tangent to the surface at a hole in question. You can add two mate to center points of a nut on the axis then constrain the face of the nut to the work plane at that hole. Its a lot of work.

 

Do you need these in the model for some reason or is this just an exercise. I know you need the part.

Hmmm ... not sure what you're meaning exactly with the creation of "some work axis" ... what are you using to make this work axis? If I can get a work axis through a hole, then I think I'll be home. Actually, it will work with just work points on the hole "centers" ... cos then I can tangent mate the face of the nut to the curve of the flange ...

Well, the assembly drawing needs to detail that each nut is there as shown and welded fully around with 6mm fillet weld. I know this, but we want to explore the option of getting these components made and assembled elsewhere, hence the need for the details inthe drawings to be precise and clear ...

The picture i posted with the projected points wont work because you have holes there and no surface. You would need to create an offset surface(zero offset) and do a boundary patch matching the curvature of the piece, then project points to that surface.

In your part file I made your original sketch visible and used the center point of each hole and the Xaxis as a reference to create the new work axis for each hole. The only issue that comes up is the axis is inline with X and not with the direction of the hole after the part is bent. If you place a constraint between a center point on your nut and the axis, then a constraint between a created work plane and your nut it would work out. Really there are a few ways around it but I dont know if the end result will really be what you want.

In the real world, how will you hold these nuts in place for welding? are you just going to set them there or will you bolt through the other side to hold them down.

Well, I had the entire thing done including placement of the nuts but then couldn't get it small enough to attach here.

Backtracked removing as much as possible but still couldn't get the file size down enough.

Maybe you can tell from history tree. I show two different methods of creating axis/workplane for mating the nuts.

These are called in-line work features in Inventor create by right mouse button selections after selecting workplane/axis/point commands. The idea is to get an axis perpendicular to the surface at any particular point on the surface. Then a workplane can be defined by that axis and point. (perp to the axis at point at surface)

The ring (including holes) is split (wrap sketch to cylinder) from surface and then Thicken.

Hello JD. Thanks again for your efforts. Can you expand your entire tree for me?

This is my train of thought so far as to what you are doing - so tell me if I'm on the correct path. ExtrusionSrf1 is the curved cylinder surface. Sketch2 is the 2D sketch with the 645OD, 550ID, and 580PCD, 11 holes 14dia. 3D Sketch1 is the projection of Sketch2 warped onto the ExtrusionSrf1. I can not work out what Split1, Split2, Split3, Split5 is doing - I presume you are using 3D Sketch1. I can't seem to select more than one geometry to do the split ... Or more to the point, I don't even know how to use Split (properly)! What does Split feature do? Can you trim away the excess surface so you just have the ring surface remaining?

Hang on ... let me go though the help files for Split to see what it can do ...

Still working on it ...

OK ... I got the hang of Split ... so what I've done is split the outer circle - split1. Then split the inner circle - split2 (now leaving the ring). Then how did you get all the holes in one split - if that's what you are doing? Else, there will be a split for every single hole (11 hoels) ... to leave the ring surface. But you only have two additional split functions ....

Or ... did you only split 2 holes to show the two exmaples?

Ooooo! I think I got it!

One last question ... why "in-line work features" as opposed to create point, create axis, create plane? Is it just to keep the tree simpler?

Ooooo! I think I got it!

 

One last question ... why "in-line work features" as opposed to create point, create axis, create plane? Is it just to keep the tree simpler?

If you were to create a plane, point or axis down the tree it would fall after the current feature. If these references are to existing work planes or points... these in-line features will fall into a parent/child relationship in the design tree. I think you nailed it. Trying to keep the tree simple. It will also help you find the relations later. For instance if you created plane20 as an offset plane of the XZ plane, later on you may not remember which plane you used as the reference. In your case since you will need multiples it will keep everything nice and clean and be easier to figure out what is referenced to what later on.

Or ... did you only split 2 holes to show the two exmaples?

Yes, I only had the two holes split. I was trying to get the file size down small enough to attach here. Sounds like you got it figure out.

BTW - looks like you are really catching on to this stuff much faster than most. Good job.

One thing I might do is create the mating parts (except for the nuts) as a multi-body solid and then on the Manage tab push out the individual parts and assembly. This ensures everything fits together ( I was a little unsure of your resulting radius using the Bend Part command in your first attempt). Keep in mind that when you wrap those holes (physically bend the part) that the holes close up a bit - make sure you have enough clearance for actual assembly of real parts.

Yes, I only had the two holes split. I was trying to get the file size down small enough to attach here. Sounds like you got it figure out.

 

BTW - looks like you are really catching on to this stuff much faster than most. Good job.

 

One thing I might do is create the mating parts (except for the nuts) as a multi-body solid and then on the Manage tab push out the individual parts and assembly. This ensures everything fits together ( I was a little unsure of your resulting radius using the Bend Part command in your first attempt). Keep in mind that when you wrap those holes (physically bend the part) that the holes close up a bit - make sure you have enough clearance for actual assembly of real parts.

Hey JD. Thanks for the complements. There are many similarities between Inventor and ProEngineer and SolidEdge ... so I guess that makes life easier.

Plenty of clearance - M12 nuts/bolts and the holes are 14mm diameter. The curvature is almost "flat" considering these dimensions.