In Inventor I know its possible to make a series of equally spaced holes around the surface of a cylinder, but how? When I try Inventor won’t let me select the curved surface of the cylinder.
Try in the browser window on the bottom left clickint the plus in front of the origin folder. Then select features in the panel bar. Then select the Work Plane tool. Then select the plane you want under the Origin folder in the browser. Then click sketch and you should be able to use that plane.
That one I learned from Clark Gilbert on 45.
“of 45” mentally, not physically anymore 
The easiest thing to do would be to make one hole then “Revolve” it around the surface of the cylinder.
Ya i know how to make stuff “revolve” around a flat surface, but i don’t know how to start a hole on the curved surface of a cylinder.
*Originally posted by James114 *
**Ya i know how to make stuff “revolve” around a flat surface, but i don’t know how to start a hole on the curved surface of a cylinder. **
You need to make a work plane that’s tangent to the cylinder. Then, create a new sketch on the plane and draw your hole. The hole will then cut into the cylinder.
If you’re lucky, the intersection of two of the origin planes lies along the center of your cylinder. In that case, create a new work plane by clicking on one of the origin planes and dragging it away – it’ll ask you for an offset distance. That distance should equal the radius of your cylinder.
If you’re not that lucky, you can fudge things a bit – but how much depends on how accurate you need the whole depth to be. To do that, just drag a new work plane out beyond the edge of your cylinder. The features you create on that work plane will still affect the cylinder.
Then, create a circular pattern of that hole around the rest of the cylinder.
That sounds good, but when I have had to make a series of hole in a cylinder, I have used the polygon tool, so if I need 8 holes I make an octagon, and then make the holes uniformly on each of the 8 sides. Then create a circle at the base of the octagon and extrude away the excess material.
*Originally posted by James114 *
**That sounds good, but when I have had to make a series of hole in a cylinder, I have used the polygon tool, so if I need 8 holes I make an octagon, and then make the holes uniformly on each of the 8 sides. Then create a circle at the base of the octagon and extrude away the excess material.
That works, too. Of course, it’s no good to you when you’re adding holes to a pre-existing cylinder 
Thats true, but i normally make all my own stuff from scratch unless its really complex
I want to place holes around a cylinder as discussed in this thread, but I need to make them parametric, so that I can slide them around after drawing them, both along the cylinder axis and in azimuth. I do not need to change the number of holes after drawing them.
This seems to contradict an Autocad paradigm, that one establishes a sketch plane which is not adjustable parametrically, and works parametrically in it. Is my impression correct, and does anyone know a workaround?
For example, I can put a sketch or work plane perpendicular to the cylinder axis, but I don’t know how to set up an adjustable dimension between that plane and the cylinder base. Further, I don’t know how to make holes without a work plane perpendicular to each hole, at least perpendicular to the first hole of an array of holes. And I don’t know how to set up an adjustable angular dimension to the first hole of the array.
I’m using Mechanical Desktop 2004 DX, but I’m not wedded to it, and if someone convinces me that this is easy in Inventor, I’ll learn enough of that to do the job.
Thanks.
Jim
I use AutoCAD 2002, and what I believe you will want to do in CAD 02 is extrude a circle of desired diameter to desired height, and then create a negative cylinder the size of the hole that you want in the original cylinder, then array the negative around the original at 45 degrees increments. Then you can subtract the negatives from the original and have holes in the original cylinder.
sarcasm That’s just my opinion, not like I do CAD just for the fun of it or anything. /sarcasm
Squirrel
My AUTOCAD is pretty rusty, but here’s how I’d do it in Inventor:
- Construct the first cylinder by extruding along an axis. For convenience I’ll use the Z-axis.
- Construct a work plane that passes through the Z-axis and at an angle to the Z-X plane. Call it 30 degrees.
- Create a sketch on the work plane. In the sketch, create a circle of the desired hole diameter and center it on the Z-axis. Project the bottom of the cylinder onto the sketch plane. The resulting line should be perpendicular to the Z-axis. Dimension from the projected line to the center of the circle.
- Extrude and subtract the sketch with the circle. Be sure to extrude farther than the radius of the tube.
- Use the circular pattern command to create multiple copies of the hole rotated around the Z-axis.
If you want to change the height of the holes from the bottom of the cylinder, change the dimension in the sketch. If you want to adjust the azimuth of the first hole, change the angle on the work plane. If you want to change the number or spacing of the holes, edit the circular pattern command.
ChrisH
Jim,
In Mechanical Desktop you should be able to generate the holes the same as you would in Autocad but with “associative” properties. Those objects should be able to move with respect to other objects in the drawing and the dimensioning should also autoupdate to reflect changes.
In Autocad I would set a UCS that is perpindicular to a tangent on the cylinder. (This is a simple operation which is easy to see if you are using a 3D view.) Then draw a cylinder of the size needed for the holes in the first cylinder with one end inside and the other outside of the first cylinder. You now have two cylinders intersecting each other. Using polar array with the center of the first cylinder as your center point of the array, generate a number of cylinders that matches the number of holes you need. You now have one cylinder that is pierced by several other cylinders. Now using the “subtract” command, use the arrayed cylinders to cut holes in the first cylinder. All of the arrayed cylinders will disappear leaving the holes you need.
I would block the polar array objects first. That way you can use the block to fill in holes if they don’t appear where you want, (use the “Union” command) and then place the object whereever you need the new holes.
Al,
Now you did it - forget that electrical stuff - you’re on the mechanical design team next year!
Raul
Raul,
That’s Autocad, not Pro-E
I offered before but NOOOOOOO! So I stay on the electrical team.