Large array, best practice

[NigelHay]

The attached .ipt is a ceramic anode, it's a square ceramic plate with an array of gold pads on both sides. On this one the array is 64x64 both sides. We all know that Inventor hates large arrays. I'm trying to create the next iteration of this anode which is the same ceramic size but the gold pads need to be smaller & in arrays of 128x128.

I've tried following this same procedure as the attached, creating 1 pad & arraying that but Inventor just gives up. I've also tried creating the array in the sketch thinking I could use the split face command after but Inventor fails in creating the sketch array.

Can anyone suggest a more efficient way of creating these parts? Be aware that, if you open the attached part, Inventor might be very slow to respond or even crash.

Inv. build 271, release 2023.2.

Win 10 Pro 64 bit.

Intel core i9 12th gen.

64Gb RAM.

NVIDIA RTX A4000 16Gb.

[Frederick_Law]

Best is don't.

Use Appearance to make it looks like its there.

If you have to, maybe split into smaller arrays.  Suppress them until you need them.

[NigelHay]

I sort of do that with the current design, I use model states to supress the arrays in the assembly so that it does not slow things down. Maybe I could get away with just showing a small section of the array in one corner.

[NigelHay]

I've tried various methods of filling the anode surface with the full 128x128 arrays of pads. I've crashed Inventor several times on the way, every time I tried to fill the whole area. What I have settled on for now is to create a smaller 20x20 array in one corner then array that pattern 4 times around the Z axis so that I can check the symmetry. This is sufficient for now to allow a drawing to be produced with the detail dimensions.

[johnsonshiue]

Hi Nigel,

There isn't anything wrong with creating exact geometry of the intended part. But, I agree with Frederick, I don't see a point making such massive pattern of geometry. My personal preference is to create geometry only when it can be dimensioned and it needs to be dimensioned in the drawing. For surface texture, cosmetic feature, there are better ways to represent it.

Many thanks!

[3D4Play]

FWIW, I was able to change the first rectangular pattern to 128x128 without any noticeable delay. However, I was going  to try and mirror it for the other side, but that choked Inventor. It also brought up another issue: the little message in the bottom left hand corner: "<esc> to Cancel Executing Create Mirror Pattern Feature" (see screensnip). Pressing <esc> once - or any number of times - has no apparent effect, unless you're willing to wait (in my case) about 23 minutes and 37 seconds before "The operation is canceled" popup happens. IMHO, something's wrong with the priority given to the <esc> key.

[NigelHay]

Much the same as my experience, every time I tried to fill the whole pattern, Inventor said no.

[NigelHay]

There are times, not necessarily in this instance, when a complete large array is required in order to supply the data to manufacturing, either as a STEP file or DXF depending on the process. Unfortunately, our particular business is based around devices that use holes (3µm - 10µm) in large arrays with corresponding electrodes so this is something that will keep occuring.

[WHolzwarth]

As an alternative I've tried patterning a separate solid, but centering doesn't work.

[Maxim-CADman77]

@johnsonshiue 

What can Autodesk recommend for those who need to build sheetmetal part with numerous cuts patterned that is expected to be DXF-exported and then cut with laser, plasma or alike machine-tool?

[NigelHay]

Maxim, I've had this trouble in the past, we know Inventor does not get on with large arrays. I've got round it by having a smaller patch of the arrayed pattern in one area of the sheet & having the supplier reproduce it to fill the sheet. Would be worth talking to your supplier to see if that is possible.

[Frederick_Law]

---

@Maxim-CADman77 wrote:

@johnsonshiue 

What can Autodesk recommend for those who need to build sheetmetal part with numerous cuts patterned that is expected to be DXF-exported and then cut with laser, plasma or alike machine-tool?

---

ModelState

Only do the large pattern in the MS for flat.

Use other one for drawing and assembly.

At current job, we punch pref panels.  We only show outline of the pref area.

Even the punch program has trouble processing all the hole.

I have to manually G-code the pattern.  Good thing it just rectangle.

Two 72 x 57 sq holes.

[IgorMir]

In such a case - I would create only a fragment of the needed array in Inventor. Create a Dxf file from it and finish it off in AutoCAD. The DXF from AutoCAD will be the file you upload to your laser cutting machine. Or whatever the machine you use for making the item.

Cheers,

Igor.

---

@NigelHay wrote:

There are times, not necessarily in this instance, when a complete large array is required in order to supply the data to manufacturing, either as a STEP file or DXF depending on the process. Unfortunately, our particular business is based around devices that use holes (3µm - 10µm) in large arrays with corresponding electrodes so this is something that will keep occuring.

---

[3D4Play]

Yes, that's a workaround, but relying on a second application just to complete an array is an expensive “right tool for the job” proposition - I don’t have a $2k USD CAD application just lying around, waiting for someone to need a workaround. I walked away from AutoCAD back in 2004 and never looked back. My expectations for this newfangled 3D modeling application are quite high by now. 😉

[IgorMir]

Well, it is true. But we shouldn't forget that even with available rail roads we still need wheelbarrows. Every now and then, at least. 🙂

---

@3D4Play wrote:

 I walked away from AutoCAD back in 2004 and never looked back. My expectations for this newfangled 3D modeling application are quite high by now. 😉

---

[Maxim-CADman77 · Accepted solution]

@NigelHay 
I can't reproduce the issue that you call "Inventor just gives up" on the IPT you've posted.
Firstly I've created the numeric User Parameter "LinearMultiplier" with value = "2ul".
I then reduced the square side size of those sketches under Extrusion2 and 3 (../LinearMultiplier)
And finally I've made appropriate changes to both patterns:
 - set 'Distance' instead of the 'Spacing'

 - changed Distance parameter (to 63 * <Spacing value>) 

 - set new instances count (.. * LinearMultiplier)

The result (see attached) I believe is what you were intended to get (I've used the move-EoP-marker-UP trick to reduce the file size. You need to move EoP-marker to the bottom after IPT open. For me all feature un-suppressing takes about 40sec).

Yet I still believe Autodesk should provide some further improvement regarding Large-patterns as Optimized option (that you've used in this model) is not applicable in some other cases.

PS:
Inventor warned that the default memory limit (1024Mb) for Undo is not enough and suggest to increase it and I've accepted this.

PPS:
I use Inventor 2023.3.1

[NigelHay]

Maxim, that works nicely, thanks. Now I just need to spend a bit of time understanding exactly what you did. I had always thought that Inventor failed because of the excess number of facets generated by a large array but your solution shows that is not the case.

[Maxim-CADman77]

Just in case:
To get 256x256 pattern you need to change value of 'LinearMultiplier' to '4' (for my PC it takes about 7 minutes to rebuild the model)

[NigelHay]

Thanks Maxim, when I get a bit of time I will study your method. Luckily, it only takes about 20s to regenerate on my PC.

[aurel_e]

I think what might have made the difference is that
"- set 'Distance' instead of the 'Spacing'"

Probably the "Distance" pattern for some reason performs better.