Placing at a compound angle

[JamesBarlow]

This one is kind of hard to describe, but if you have ever done this should know what I'm asking.

What I am trying to make is a machine base with a drip tray that is angled twords one corner to collect coolant.

The base is made of four plates creating a squate (Imagine a box with no top or bottowm.)

In this box I would like to place a plate that is angled twords the rear left hand corner to allow coolant fluid to be collected at the back of the machine.

The plate is cut as a parallelogram so all four sides will meet up with the four sides of the box.

It took me the better part of a day to figure this out and I'm still not happy with my solution.

This is what I did.

I picked 3 corners on the plate and made a connect with 3 faces in the box. The parallelogram forces the plate to sit at a compound angle. I then connect a line on the plate to a point on the top of the box to get my depth of the plate from the top.

By playing with the geometry of the plate I can adjust the angles of how the plate sits.

These seemes to work, but it's a very slow and time consuming way of putting the plate in. Since the plate is being welded, water tight, in place I only need to be close, but I can't help feeling there is a better way of doing this.

If anyone has advice of suggestions I would really appreciate it.

 

[PatCouture]

Why don't you simply do your bottom plate in the context of the assembly.

If you have your four side already, with the exact shape of where you want to collect the fluid, I don't see any problem doing an In place part so that you are able to create a reference plane by 3 points at the bottom of the boxe and then doing a tab by including the geometry.

Maybe I don't understand correctly what you want to do, but the way I see it it's not complicated. It's way more complicated to do the base plate with a bend in it between two corners.

I hope this help.

Patrick

 

[fwc]

Hi

I created the Tab on a reference angle which is reference to x-y plane. Then project the cutout (the parallelogram) from x-y plane. With this I can mate the sides of the parallelogram to the sides of the box and I used the x-y plane for the 3rd constrain.

Hope this helps.

 

[kjoiner]

James,

Here's my attempt:

1. Create a "box" with no top or bottom, just 4 sides using contour flange.
2. Place this box in an assembly.
3. Create in Place a new sheet metal part. I called my the "baffle"
4. In the "baffle" I insert part copied the top and bottom faces (edges) of the box. I then offset the top edge to account for the thickness of the new "baffle"
5. In the top view I sketched a line across the corners of the inserted edges.
6. I created a surface using this line. (It's easier and more flexible than creating a plane for the next steps.
7. I made a new sketch using the surface as my plane for drawing
8. I drew a diagonal line from the top corner of the upper edge across to the bottom corner of the bottom edge ( of the inserted faces)
9. I created another surface that extends symmetrically out beyond the edges of the inserted faces.
10. Using the project curve, I projected the inside chain of lines down onto the angled surface
11. Because I had created my "box" using a contour flange and the ends can't touch, I created a keypoint curve to fill in the gap.
12. I then used the tab command to create a flat plate of the desired metal thickness.

There is probably a more elegant way to do this, but this method should let you change the size of your box and the baffle should adjust accordingly. I tried creating a plane on my first attempt, but I used a 45° rotation and as soon as I changed the box dimensions out of square the baffle failed.

Kyle

 

[JamesBarlow]

I feel more confused now then before.

I think what I didn't explain is that I'm not using the sheetmetal function.

The box is made of 1/4" think plates which are welded to create the box.

The baffle, as Kyle called it (I'm calling it that now as well) is another 1/4" plate that is cut and placed.

Here is were I am loosing it with what everyone has suggested.

The plate, in this instance, is located with it's highest point about 8 inches below the top of the box. From there it angles about 5deg from right to left, and 5deg from front to back. The box itself is 24" high, so the plate is located in the limbo land between end point and mid point of the box side so I can't grab anything to locate it.

I hope this helps some.

 

[PatCouture]

ah ok! I didn't see it that way.

Maybe you can draw some sketches on different sides of the box just to get each corner exactly where you want.Then you would be able to create a reference plane with 3 point to create the botton of your box.

I hope this help.

Patrick

 

[kjoiner]

James,

Here's another quick try. I have not drawn this so I can't say this will work for sure but here it goes.

Sketch a line that handles the 5° tilt from front to back. Then place a plane that is perpendicular to the end of that line. Create another sketch using that plane that is 5° left to right. Then create a surface using that line, trim it and thicken it.

Kyle

 

[PGJ]

I just glanced at the above and found it an interesting problem as I'm an ex machine tool man myself but I'm not a SE person, I use Solidworks. The first thought I had was to take the machine base box profile and use it as a cutter. Position the Base Plate (any size larger than required) at the compound angle and perform an Extrude Cut which will give you an exact profile for the Base Plate, however, cutting this in real life maybe another problem. As you know there are other ways of designing a machine base to collect coolant but that's another issue.

 

[beachcomber]

In a new part file, create an open-ended extruded surface to represent the inside of the box.
On one side create a sketch line for the front/back slope of the bottom plate.
On the back face create a sketch line for the sideways slope of the bottom plate.
Now create Plane No.1 by 3 points with the origin at the corner where the 2 sketches meet.
Create Plane No.2 parallel to this one, offset by the thickness of the bottom plate.
Create an intesection curve between each plane and the suface.
Create a sketch on Plane No.1 and include the intersection curves that lie on that plane - this will be the profile for the bottom plate extrusion.
Now create a sketch on Plane No.2 and include the intersection curves that lie on that plane.
Create a solid using the sketch on Plane No.1 - use Plane No.2 as the extent.
Create a cut using the sketch on Plane No.2 - don't forget to set the side to be cut or you will just end up with a thin bit on 2 sides.
You should be able to position this plate using connects, or by the surface, or reference planes which will be located at one inside corner of your box.
In this case the plate will not be associative with the box - if you want to do that, let me know.

 

[fredericmenage]

Hi,

My try:

1/ make your box without top and bottom in an asm
2/ create in place a new part (doesn't matter where)
3/ close and return. RMB / occurence properties : choose a position and orientation for the center and the planes of your angled plate
4/ edit that part. Insert / Interpart copy for the 4 inside walls
5/ create an extruded surface using a line extending way past the surfaces on the plane x-z (or whichever is appropriate), use a symmetric extent extending way past the surfaces as well
6/ give a thickness to that surface (thicken)
7/ boolean (x4) (subtract + outside direction) that plate using the interpart surfaces.
8/ if wanted, add a cutout on the top face by including the appropriate edges to correct the edges of your plate at 90 degrees

NB: if you need to edit the plate go to occurence properties in the assembly to change the compound angle. Then hit 'update all links'.

Fred