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

[IgorMir]

Hi Donald,

Looking at the flat pattern - the holes are on the angle to the face. How that is going to be produced? As for the bolts following the hole pattern in assembly - you can link parameters from the part to the assembly and use them to control the bolts' pattern.

These are a few things which came to mind.

Cheers,

Igor.

[jhackney1972]

You show pictures of an assembly and the one file you attached opens with a resolve link problem.  I believe you missed something in your Pack and Go that you need to send out for others to help you.  Please zip you Pack and Go so it will be easy to manage.

[donaldleigh]

Hi @IgorMir

The holes in the flat pattern will not be cut on the angle. We will produce a DXF of the face only.

but thats one of the issues I have. How do I make the holes perpendicular to the face so that the bolts in the assembly are shown in the correct way in the assembly??? 

@jhackney1972

I have linked the number of holes in this spigot to the retaining Ring that is on the outside. Attached is the file without the link

[IgorMir]

Hi Donald,

It is actually an interesting model. Here are some files (IV2018). I have simplified your model a bit but the end result for the hole's array is still the same. They are all tilted to some bias angle. As can be seen in Part1.ipt - the Work Axis 1 is parallel to the XY plane. Yet the Work Axis 2 is tilted substantionaly. I couldn't pinpoint the reason for it. I hate to suggest but that might be some deficiency in Inventor itself.

Now, to the assembly. All the bolts in the array are tilted as well. The first bolt is fully constrained.  Yet it seems that the arrayed parts do not obey Tangent and Angle constraints at all. I would be very keen to hear from anyone the reason for it.

Thank you,

Igor.

[TheCADWhisperer]

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@IgorMir wrote:

...I couldn't pinpoint the reason for it. I hate to suggest but that might be some deficiency in Inventor itself.

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I don't own a rar extractor to check your file, but in the original file 

Cut1 is done incorrectly

Rectangular Pattern1 is done incorrectly.

I don't have 2014, so if I made the corrections - the OP would not be able to see how it was corrected.

Tip: Helix

[IgorMir]

Thanks for joining in. Here is a stand alone file.

Cheers,

Igor.

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@TheCADWhisperer wrote:

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@IgorMir wrote:

...I couldn't pinpoint the reason for it. I hate to suggest but that might be some deficiency in Inventor itself.

---

I don't own a rar extractor to check your file, but in the original file 

Cut1 is done incorrectly

Rectangular Pattern1 is done incorrectly.

I don't have 2014, so if I made the corrections - the OP would not be able to see how it was corrected.

Tip: Helix

[TheCADWhisperer]

The start position should be at the center of the hole and the path is a helical curve.

All hole axis will be parallel to the XZ plane.

[IgorMir]

I might be overlooking something obvious here but so far - no dice. Here is a quick attempt with the helix. Still the same outcome.

[TheCADWhisperer]

I used the Coil command to create helical surface.

[donaldleigh]

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I don't own a rar extractor to check your file, but in the original file 

Cut1 is done incorrectly

Rectangular Pattern1 is done incorrectly.

I don't have 2014, so if I made the corrections - the OP would not be able to see how it was corrected.

Tip: Helix

 Hi @TheCADWhisperer thanks for your input. As I have 2014 are you able to take a screen shot of the browser so that I might be able to work out how you do it. I'm not sure how else you can do the cut and pattern. remember that I also need a flat pattern.

Im hoping also that our company will be going to the latest version soon so if you can still send it as well maybe I can look into it then.

I will look into the helical curve also.

Thanks

Donald

[IgorMir]

Good morning The Cadwhisperer

I don't think the coil command is a solution here. Yes, the holes axises are parallel to the XY plane but the vertical distances from the centres of the holes to the top edge are all different. That's what I got anyway. And in the image you have posted earlier it appears to be the case as well. Could you please take a screen shot of the flat pattern and post it here?

Thanks,

Igor.

[IgorMir]

Good morning everyone,

I have spent some time looking for the best solution for the task at hand. And unfortunately - couldn't find a workable solution in Inventor. Yet to make that part in real world is not an issue, really. It can me made on a simple milling machine.

Attached are three parts for anyone who wants to have a look at it.  IV 2018 files.

Part1 utilises a rectangular array for the holes. The holes follow the slop, but their axises are all tilted. They are not parallel to the XY plane. Except for the very first hole. As a result of it when the part is placed into an assembly - Pattern Components using Feature Pattern option becomes useless.  All the bolts will be seating on an angle to the outer face, which is wrong. BTW - Inventor seems to ignore Tangent constrain of the bolt's face to the outer face of the part when using Pattern Components tool. 

Part2 is done with Unfold/Refold command to get the holes axis parallel to the XY plane. It is achievable but after the refold Inventor is incapable to introduce a Work Axis to any of the hole. It is understood, since the hole gets deformed. 3D Sketch comes to the rescue in order to create some auxiliary geometry. What I can not understand is - why the Point in a 3D Sketch is still green while it is constrained to the middle of the line? What other degree of freedom does that point have? Besides - I couldn't figure out how to Pattern Components in assembly using Feature Pattern option. It is just not there.

Part3 is done in old fashioned way.  All the holes are parallel to the XY plane. Naturally - on the flat pattern they are all ellipses - but that's expected. There is no problem with constraining bolts to any of the hole but editing the part will trough the assembly constraints ballistic. Not to mention that creating that part in Inventor is a pretty tedious task in the first place.

The idea of using a 3D spiral for the Hole Pattern direction is not practical either. While the holes are parallel to the XY plane - the vertical distances from the slopped edge are all over the place.

That's all I can say about that part for now. Comments are welcome.

Cheers,

Igor.

[donaldleigh]

@IgorMir and everyone else Thanks very much for looking into this. I have also tried both your part 1 & part 2 and come up with the same problems. I think the issue could be solved if the pattern component in the assembly can keep the same axis as its rotated, but there is no option for this. Similar to the options available in the pattern feature of the part.

In reality the part is manufactured in these steps

1. Flat pattern is laser cut with holes.
2. Rolled to the desired ID and welded at join

Yes this will distort the holes but that's not an issue.

Donald

[IgorMir]

Then it would be fair to say that Inventor is an inferior software for this particular task.

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@donaldleigh wrote:

@IgorMir and everyone else Thanks very much for looking into this. I have also tried both your part 1 & part 2 and come up with the same problems. I think the issue could be solved if the pattern component in the assembly can keep the same axis as its rotated, but there is no option for this. Similar to the options available in the pattern feature of the part.

In reality the part is manufactured in these steps

1. Flat pattern is laser cut with holes.
2. Rolled to the desired ID and welded at join

Yes this will distort the holes but that's not an issue.

Donald

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[WHolzwarth]

Have a look at the attachment (2014 IPT). Perhaps that is the way to go.

But there seem to be two bugs present from Inventor 2014 up to 2019.

1.Refolding changes stationary plane of the part, and after that the final mirror fails.

2. Mirror is possible after suppression of Thicken1, but this way the Rip needs to be applied as a final step.

@Anonymous: Are you watching?

[IgorMir]

Hi Walter,

If you create an assembly, put this part into it, insert a screw into the first hole - can you pattern the screw using Feature Pattern option? 

Regards,

Igor.

P.S. As for the refold changing orientation of the part in space - I have risen that question with Johnson not so long ago.

As you have mentioned - the problem has been known since IV2014. Say no more.

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@WHolzwarth wrote:

Have a look at the attachment (2014 IPT). Perhaps that is the way to go.

But there seem to be two bugs present from Inventor 2014 up to 2019.

1.Refolding changes stationary plane of the part, and after that the final mirror fails.

2. Mirror is possible after suppression of Thicken1, but this way the Rip needs to be applied as a final step.

@Anonymous: Are you watching?

[WHolzwarth]

Hi Igor,

in theory placing of workpoints in the hole centers after refold and after that workaxes - perpendicular to the surface in that position - would be possible.

I used this method:

In unfolded part I placed short lines (Length=hole diameter) tangent to the guiding curve. After refold these curves were wrapped back to the round geometry. But sad to see, that their position didn't match with the holes (see picture).

If this would have worked reliably, then there are two ways possible (perhaps more, too):

a) Workplanes at both ends of the projected segment -> Hole axis through workpoint at their midplane

b) Workpoint at one end of the projected segment, after that 3 instances of rectangular pattern at segment curve length.

So far theory. Real life shows that Inventor (tried it with 2019) is not perfect.

On the other hand: A cylindrical  surface cut with an angle results in most cases in an ellipse section. I can't imagine any good bolted connection with another part all along the circumference.

[WHolzwarth]

Back again now: There's been a bug in my brain with respect to the bad projections. Why?

Unfold-Refold depends on the k-factor settings. If I'd wrap to an internal face with distance k*thickness vs the outer ring, things should be ok.

Not tested, only imagination.

[IgorMir]

Hi Walter,

I take it you didn't have time to try to create an assembly using your part yet.

Cheers,

Igor.