Hole Pattern on sloped surface

[donaldleigh]

Hi all

Can someone please let me know where i'm going wrong. we have Inventor 2014

I have a Sheet Metal part rolled spigot with the front face cut on a 1:16 slope. We then need to drill a series of holes around is keeping all the holes 15 mm from the sloped face (Work Plane1). Each hole should also be drilled parallel to the rear face (XZ Plane). 

as the hole pattern goes around the spigot the hole don't keep parallel to the rear face (XZ Plane).

I know you can use the fold/unfold but the issued with this is that in the top level assembly the Component Pattern would not would and I would need to insert each bolt.

I have attached the spigot and also an image of the top and bottom with the bolts.

 

kelly.young has embedded your images for clarity.

Cheers

Donald

[WHolzwarth]

Good morning Igor,

not right now. New attempt in about 12 hours.

Is placing only two screws enough?

[IgorMir]

Good morning, Walter;

No,  placing just two screws is not enough. The idea is to use Feature Pattern function in Assembly Pattern.

I hope - maybe you find a workable solution. I personally got involved into this topic purely out of curiosity. While working on a solution for the OP - I have came to a conclusion that Inventor is not capable of handling this type of the geometry in the way so it can be used efficiently in follow up assemblies. Yet I could make a smaller version of that part in my workshop in less than two hours.

Kind Regards,

Igor.

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@WHolzwarth wrote:

Good morning Igor,

not right now. New attempt in about 12 hours.

Is placing only two screws enough?

[johnsonshiue]

Hi Guys,

I am sorry that I did not follow this thread as much as I should. I will take a look and get back to you with my findings next week.

Many thanks!

[WHolzwarth]

In the meantime I can show an intermediate result, Johnson.

But what's the best way for placing real screws in an assembly, on the dummy positions?

[IgorMir]

Thanks, Johnson.

We look forward to your solution. 🙂

Cheers,

Igor.

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@johnsonshiue wrote:

Hi Guys,

I am sorry that I did not follow this thread as much as I should. I will take a look and get back to you with my findings next week.

Many thanks!

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[IgorMir]

Hi Walter,

It seems - you are trying to introduce a dummy extrusion into the model with the idea of using it to constrain the bolts to it in the assembly. If I am right in my assessment - than there are two questions for you. First - are those extrusions round? Second - how do hide them in assembly?

I did try to introduce the dummy extrusion in Unfolded model. If the extrusion is not crossing the face of the part - it is not following the part after Refold. If the extrusion overlaps the face - it gets squashed up just like the hole does. And it make no difference that the extrusion has its own parameter, extrudes both ways or just to one of the directions.

I recon - Autodesk should put us on payroll so we can sort that problem out!

Cheers,

Igor.

[IgorMir]

Hi Johnson;

Here is one more thing which I can not pinpoint the reason for. In the attached image the measured angle reads 6.25°. But the controlling sketch shows 6.17° Where the discrepancy is coming from?

Thanks,

Igor.

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@johnsonshiue wrote:

Hi Guys,

I am sorry that I did not follow this thread as much as I should. I will take a look and get back to you with my findings next week.

Many thanks!

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[WHolzwarth]

Hi Igor, I'm answering between the lines.

@IgorMir  schrieb:

It seems - you are trying to introduce a dummy extrusion into the model with the idea of using it to constrain the bolts to it in the assembly. If I am right in my assessment - than there are two questions for you. First - are those extrusions round? Second - how do hide them in assembly?

1. Extrusions are cylindrical shape

2. Hiding perhaps by placing cylindrical surfaces instead of solids

I did try to introduce the dummy extrusion in Unfolded model. If the extrusion is not crossing the face of the part - it is not following the part after Refold. If the extrusion overlaps the face - it gets squashed up just like the hole does. And it make no difference that the extrusion has its own parameter, extrudes both ways or just to one of the directions.

That's the problem: Cylindrical shapes in flattened parts become non-cylindrical after rounding. Cylindrical holes in rounded parts can't be made easily in flat pattern; they would have been done non-cylindrical there. No way out.

Looking at your file above, thanks for pointing me to the Center Point of Loop of edges feature. I wasn't aware of that; using it my sample can be done with fewer steps.

IMO the used pattern in your file has precision problems. The guiding curve is the outline of the unfolded part; an offset curve would give better results. You can see slight differences in measurements of hole centers vs the outline.

The angle difference may be caused by this setup of the guiding curve, combined with the starting point at the low end of the flat part. The angle measurement is done at the high end; all precision errors are summed up.

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[IgorMir]

Hi Walter,

We do spend time on this one, don't we? 🙂

Anyway,  here it is in reply to your comments.

1. How did you array the cilindrical extrusion so it is still in round shape? When I tried to array following the tilted curve - they all do get tilted as well. Just as the holes do. Which is not acceptable. Trying to introduce the extrusion in the unfolded model - if it is a surface, after the refold it stays where it was in the unfold mode. Just like the Work Points do. None of them do follow the model.

2. For the precision error in my file. In Sketch1 I dimensioned the length of arc, not the chord of the arc. And that dimension is introduced to the Hole1 Sketch. The only explanation to that discrepancy I can offer is that in Unfolded state the material gets compressed. Hence 50 mm on the flat pattern are not the same 50 mm on the folded one. To combat this I can introduce a pilot hole prior the Unfold and use it as a reference for the follow up holes. Will give it a try in a moment.

Best Regards,

Igor.

[IgorMir]

Well, here is one more part to look at. IV2018. It gets more and more interesting by the minute.

Yes, the angle measurement discrepancy is sorted. Thanks, Walter. You made me think in the direction of compressed/uncompressed material. But what to do with the pilot hole itself after the array?

Please see the attached file.

Cheers,

Igor.

[IgorMir]

Ok, to combat a pilot hole issue a Split Face can be used instead. Now we have to find a way to make the bolts to follow the hole pattern on the assembly level.

[WHolzwarth]

I've used a shetch driven pattern for this, Igor. You can create a cylindrical body on the center point of the first hole, and pattern it along 3D sketch points. These points must be placed in a 3D sketch, therefore projecting of the edge-loop centers is needed.

Attached is a 2017 fileset for some pins placed on an irregular 2D sketch. I didn't test it here, but I'm expecting similar behavior being possible in this 3D sketch

[IgorMir]

Thanks, Walter but I have failed to see the similarity. Anyway - let's see what Johnson will come up with. That academical research of ours is getting out of hand, I afraid. 🙂

Cheers,

Igor.

[WHolzwarth]

So, here's the result (2019 fileset). It's not quite straightforward, but done.

Johnson's main task now would be looking for the cause of the flipping refold.

Having this completed now, I'm asking myself:

What's better? Placing the bolts with equal distances along the guiding curve, or using standard angle steps around the circle?

Answer: I'd prefer equal angles. Placed dimensions at the flatpattern would be looking better.

[IgorMir]

Well done, Walter!

Now, if you change the amount and position of holes - will the assembly array react properly to it?

Cheers,

Igor.

[WHolzwarth]

I think so.

[donaldleigh]

Good Morning all.

I hope everyone had a great weekend. On opening up my emails this morning I was surprised with all the comments on my issue. Thanks to everyone so far for this. I have really opened a can of worms.

@WHolzwarth Hi Walter, It looks like you have found a solution but We are currently only working with 2014. Are you (Or anyone else) able to convert this.

Donald

[IgorMir]

Hi Walter,

Have you tried it? My experience with sketch patterns is not that positive...

Cheers,

Igor.

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@WHolzwarth wrote:

I think so.

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[IgorMir]

Good morning Johnson;

While on this topic could you please have a look at the attached file? IV2018 format.

Work point 1 & 2 are needed to be redefined. They both were created using Center Point of Loops of Edges option. I can't select that option when redefining the points. What can you suggest?

Thanks,

Igor.

[WHolzwarth]

Good morning, Donald and Igor.

Conversion to 2014 seems not possible to me the easy way. The key for some comfort here is the Sketchdriven Pattern (SDP), accessible first time in Inventor 2017.

The only way is conversion by STEP or another format, and grounding all converted components in the imported assembly.

@IgorMir : I didn't try another setup. Perhaps not all features are changing from themselves, but the main benefit would be a trustable refold without a chance for flipping and - of course - the SDP.