Hi.
I want to make a hole that is angled 45 degress in a mould opening vertically. I have tried to sketch below how I imagine the mould parts to look like.
When doing a draft analysis it looks almost fine. I just need to get rid of the "rainbow" area in the middle and have a "clean cut" going from blue to pink with no transisition.
Any good ideas on how to do that?
Let's see if this helps.
There is nothing easy about manually making dies for injection molding or die casting. This was a good challenge none the less. The custom made extensions for doing this in Creo work the same way (extensive use of merge features). In this case, I was very deliberate with some of my choices. This is key to understand how you wish to attack each case.
In this case I used the following assumptions:
- I want a perfect circle on both sides of the sheet
- The circle is the same size on both sides (no draft offset)
- No textures will be present within the hole
- Minimal zero draft is allowed
- No slides
So this is what I came up with:
I used a series of sweeps to match ~95% of the circle perfectly (the part that has significant draft naturally).
I used the merge/cut-out feature to create the hole in the sheet. Personally, I don't like using separate dependent files, but there you go. Now that I have a good visual, I -might- be able to do this ends remove the die's merge features on the work part. Everyone has their own comfort level.
Now if I did this in the sheetmetal module, I might make the die on the fly using the surfaces. Although I prefer modeling with solid features, to make the female cavity in the die I had to merge surfaces and solidify them.
Although the questionable region looked small, it actually has negative draft that is rarely allowed although there are cases that this is done on purpose. In general, bad idea. See where the die transition must happened:
I assumed a 10 degree die transition angle (mating faces of the die); 2.5 degree standard draft on the part. the orange transition in the next image is well on the way to 2.5 degrees. the green is the 0-draft region necessary to meet my "perfect circle" goal.
Here you see the analysis on the die (both dies are identical)
The green triangle is the region created as a divergence of 2 sweeps. The majority of the circle sweep is normal to the curve (the scribed circle), but the transition was swept at a normal of the pull direction. This is how the undercut was avoided.
If you have the full version of Creo 2 (not academic), I can provide the parts to see how I got there. I need to do some cleanup as I got a bit messy for my own tastes. I tried quite a few iterations to get to this result. This one was the most straight forward approach.
That's what happens when you have too much time on your hands.
Attached is a clean version of the files:
Doug, you are right that approximations are easier to model and certainly easier to manage.
Do an analysis on on your simple version. You will still find negative draft in those 2 files. I was working on a similar version to simple_2 where the parting was through the hole at opposite end (skewed oval through the center; image below). It became quite complex from a modeling perspective fairly quickly as I ended up with the dreaded tangent convergence that virtually all CAD systems choke on.
Also check the boundary blend version. Although it works very much the same, it is still slightly different than the straight forward die version. The remaining interference is slightly less in the version provided. Again, it all depends on the assumption you have to apply to the design intent. I've never been one to "approximate" what I hand a machinist. I much prefer providing true intent.
Below is that alternate. Although I could make the surface to close the transition gap, due to the tangent interface on the shallow end, I could not get it to solidify. Same old problem. But the idea is sound for a simplified die.
Most likely... since the hole is on a high angle, the machinist wouldn't care about the higher post. He/she is machining the face anyway and has plenty of material to make the posts. Why not make the best feature possible. Again... not knowing design intent, it is hard to argue the engineer's choice of requirements.
I did a little more work on the alternative hole.
New assumptions:
- Through hole perfectly round at face angle.
- Minimize deformation at surface
- No negative draft permitted
- Zero draft permitted on a limited basis
- No texture in the hole
In this case, the draft is offset immediately at separation due to the high draft on the opposite face. Still more zero-draft than the original so total zero-draft analysis of the mold must be considered. No surfaces or approximations.
No separate die file ...but the work was duplicated for each half. Maybe rotational patterning would save some effort. A lot of prep work for related features. A bit more effort would reduce the feature count. A little more relation work and the hole is easily scalable (think UDF).
Creo 2.0 and STEP attached
Physical tooling view (reference - not required in model):
Hi all.
First of all thanks for your help and the attached files. It makes it really easy to understand what you mean.
I'm amazed by the quality of the answers.
Then I must say this solution is a bit more complex than imagined.
To put it into a context. A strain relief has to go through the hole, and I really can't allow much tolerance in order to keep it tight. I tried quickly to split the draft in the middle of the thickness, but I think the gaps are to big.
I think Doug's solution 4 will work quite well, though.
But again as said previously, I'm maybe doing it way more complex than it has to be. Just can't see how to simplify it when I can't allow too big gaps, other than using some side actions, which also is an option.
If you have any great ideas, feel free to write'em here
I'm sure you already looked into if you can change the angle of the mounting surface, that would help a lot if you could get it closer to horizontal. 
You can take that #4 and move the P/L sketch so that the left side is close to the bottom and the right is close to the top to get as much 'true diameter' as possible. It doesn't need to be parallel to the wall.
Good luck.
Ok, so, here's my simplified take on this:
The parting line/shutoff is extremely easy, simple, and cheap: It's flat, halfway thru the part, parallel to the surfaces you'll mate against. On either top or bottom end (in the pic), you get 1/2 the material thickness to locate the strain relief. In the center you get the whole thickness. I added 1deg of draft in the pull direction (normal to the top plane) for sheyts and giggles. From what I saw of your needs, I think this will work just fine. If you absolutely HAD to have the circle as close as possible, then Anonius's solution is what you want. It all depends on your needs.
I've included the part as well.
Have fun with it!
Here's another take on it. Very similar to what Antonius did in the "silver" model (from the pic, I can't open the models). This gives a very close approximation of the hole, with a slightly more complicated shutoff. It's funny, I first didn't understand why it "lobed" the hole (as it did in his pics too), then I realized what the VSS was doing, and think it did exactly as asked.
I was intrigued by this method for getting draft included and it worked great with the sweep. Once merged with the extrude, it leaves a little "hangnail"... a non-tangent transition between the ellipse and the circle along the edge. I created a sketched line to create the tangency on the surface and used it for a VSS between the line (origin) and the parting line ellipse (chain1). I drew a line in the section between the two "x"'s (trajectory intersections) and let it trim out that small triangle. Beautiful results as the sweep trajectory (origin) is not quite vertical so the "normal extrude" semi-circle, without draft provides nearly the same draft as the selected draft for the other half of the cut.
And yes, getting that little sketch to behave tangent to the reference can be tricky, but it works.
This is indeed a great way to ensure draft on all faces of this type of feature. ...until such time that we can extrude in a direction other than normal, that is. How is that feature coming along, PTC? 
Here's another take on it. Very similar to what Antonius did in the "silver" model (from the pic, I can't open the models). This gives a very close approximation of the hole, with a slightly more complicated shutoff. It's funny, I first didn't understand why it "lobed" the hole (as it did in his pics too), then I realized what the VSS was doing, and think it did exactly as asked.
Hangnail....
My initial sweep includes the draft in both directions. Constant normal to the pull direction.
The second extrude is along the hole direction (45 degrees), no draft, and extruded to the vertical (pull direction) plane to protect the already established surface.
A bit more work let me do a fully scalable version including the trimming of the hangnail. But I concur; all too often a mirrored/patterned feature simply fails and often fails scalability.
For Creo 2 people: See attached
BTW, ... how do you manage doing stuff when you layer hide things all the time. UHHHGGGGG! I start with empty part just so - I - have control of the layers
