Angled holes?

[[527]phil]

Hello everyone. I'm trying to make a hole at a 45 degree angle from a surface, but i can't seem to figure out who to do it. the only way i was able to do it was to make a surface at the angle i wanted, then i drilled the hole through it, but then i couldn't delete the surface and keep the hole. Anyone know how?

[i_am_Doug]

Originally Posted by [527]phil

but then i couldn't delete the surface and keep the hole. Anyone know how?

Umm, im not sure i know what your talking about..but if your useing a drill press you can tilt the platform that your piece of work is on...

~Doug

[JamesBrown]

Originally Posted by i_am_Doug

Umm, im not sure i know what your talking about..but if your useing a drill press you can tilt the platform that your piece of work is on...

~Doug

The post is in the inventor forum, I am pretty sure he wants to do it in inventor, not in real life (yet).

[Tristan Lall]

I don't have Inventor in front of me now, but what about creating a work plane at an angle to the existing surface? Then sketch the outline of the hole in the workplane and create a feature, setting the depth to whatever you need (through to reverse side). To be honest, I don't remember if Inventor will let you create a solid material removal feature (i.e. hole or cut) from a workplane in space, but it's worth a shot.

Also, since you may want to actually build the thing later, be aware that it is tricky to drill an angled hole. You'd either need a drill guide (some hard material which already has the desired angled hole), or a very stiff machine, like a milling machine and a short, inflexible bit or end mill. Even if you tilt the table of a drill press, the bit will usually walk off and make a mess.

[i_am_Doug]

Originally Posted by JamesBrown

The post is in the inventor forum, I am pretty sure he wants to do it in inventor, not in real life (yet).

Oh, right then.
I had thought I clicked Tech...
Is Inventor like Auto cad?

[Andy A.]

Creating an angled workplane in Inventor, version 10 at least, is actually very easy.

In the image I've posted below, I created an extruded block. To create the angled workplane, I first selected a face, the 'top' and then one of the edges. Inventor then prompted me to enter the relative angle of the proposed workplane. I arbitrarily used 32 degrees.

I the created a sketch on the workplane, and placed a point center by eye. Then, using the hole command, I placed a plain hole through the part using the 'through all' terminator.

I eyeballed the placement of this hole. You could constrain the placement relative to other geometry a few ways though. The nice thing about this, and any method that uses a feature, over using a boolean subtraction, as Al suggested he might do in AutoCAD, is that this feature remains adaptive and can be later changed. Changing a solid model in AutoCAD is just a pain in comparison.

You could also form a hole that follows a work axis between two workpoints, although getting a fully formed hole is a little tricky. I can go off on that if someone wants me to, but I am guessing that the angled workplane is probably adequate for what the OP was looking for.

[Molten]

The easiest way, in my opinion, would have to be the sweep command. It is a little confusing at first. Mainly because it uses two sketches. Just make a sketch with the hole drawn on it just like you would for an extrusion. Then make another sketch that shows what path you want to cut along. Then just select 'Sweep' and insert the two sketches. This should get you a near perfect cut. (It might mention a possible error about the cut not intersecting with the path but 99% of the time just ignore the warning.)

[rohit]

What I do is make 2 sketches. Draw the first one on where the hole will be. Offset a workplane to the depth of the hole and draw another circle on it. Then, use loft (shift+L) to connect the 2 circles and use the cut option and you have the angled hole!

[Molten]

I take back my advice on using the sweep command in this particular case because though you are cutting a circle, it is an ellipse on each surface. Unless you want to draw the ellipse, you can not use the sweep or loft. I would have to agree with others when they say to use the rotated work plane with extrude.

[Andy A.]

Originally Posted by Temper Metal

I would have to agree with others when they say to use the rotated work plane with extrude.

An angled work plane is perhaps the easiest, most direct approach. However, I would discourage the use of boolean subtraction (cutting a hole with an extrude command). The power of programs like Inventor and Solid works is that the models are parametric. By using a hole feature and constraining it's position with relations and dimensions, you can quickly and easily change the size, location thread treatment and depth of that hole, among other things. An extrusion is less flexible.

The rule of thumb is that if the hole is going to be drilled in some way, use a hole feature. If it is innate to the part, like in a casting or forging, use a cut hole (extrusion).

-Andy A.

[NeedMoreEngines]

Originally Posted by i_am_Doug

Umm, im not sure i know what your talking about..but if your useing a drill press you can tilt the platform that your piece of work is on...

~Doug

Lol...i was thinking the same thing. i'm like "um...it's easy."

[Madison]

Originally Posted by [527]phil

Hello everyone. I'm trying to make a hole at a 45 degree angle from a surface, but i can't seem to figure out who to do it. the only way i was able to do it was to make a surface at the angle i wanted, then i drilled the hole through it, but then i couldn't delete the surface and keep the hole. Anyone know how?

You should be able to create a new work plane that is offset 45* from the surface the hole enters into (assuming it's flat) and then create a new sketch on that plane for the hole.

[Philip W.]

Originally Posted by M. Krass

You should be able to create a new work plane that is offset 45* from the surface the hole enters into (assuming its flat) and then create a new sketch on that plane for the hole.

Creating the angled workplane would be the correct choice, but actually doing it is tricky. I'm using Inventor 9 and don't know if there's another solution for other versions. Anyway, an angled workplane must be created based on two references: an axis that it will rotate upon and a surface that the inputted angle will be based on.

Your axis is already there if your hole is on the edge of an object, otherwise, you'll have to create your own axis. You can create a line in a sketch, a work axis by two points, or a work axis by a point and a surface (it will be perpendicular to the surface and pass through the point). The surface should be easy to find.

If your hole is on the corner of an object, I would have to call you crazy, but it can be done. Ask if you need more help to do that.

[SgtMillhouse648]

Originally Posted by [527]phil

Hello everyone. I'm trying to make a hole at a 45 degree angle from a surface, but i can't seem to figure out who to do it. the only way i was able to do it was to make a surface at the angle i wanted, then i drilled the hole through it, but then i couldn't delete the surface and keep the hole. Anyone know how?

if you want to delete the surface, don't "delete" it, but right click the feature on the explorer thingy window, and supress the feature. the feature won't show up, but you will still keep the hole
good luck
malhon

[Tristan Lall]

Originally Posted by SgtMillhouse648

if you want to delete the surface, don't "delete" it, but right click the feature on the explorer thingy window, and supress the feature. the feature won't show up, but you will still keep the hole

Don't suppress it, hide it instead (visibility off). If the program is working correctly, suppressing the feature will suppress all dependent features (e.g. the hole you want to keep). Hiding it just makes it invisible.