How do I make the hole patern folow the changing patern in the slotplate?

[ErikMebo]

Hi All,

I'm trying to make the hole patern in a beam automatically follow when I change the hole patern in the slot plate. I hope the video makes it easier to understand. 

[CCarreiras · Accepted solution]

Hi!

You just have to "Use" the L Beam pattern values in the Square Beam pattern.

You have to link the pattern parameters between those parts:

When editing the Square Part, go to parameters chart and link the pattern parameters from the L Beam.

(Before linking the parameters, You have to rename the pattern parameters in the L Beam chart, something like "Pattern_Number_BL" and "Pattern Distance_BL")

Then use the L Beam linked parameters in the Square Beam Pattern.

[johnsonshiue]

Hi! Another approach is to leverage Sketch-Driven Pattern. You may create a sketch (projecting the holes to the sketch). Then pattern the slot based on the projected sketch points.

Many thanks!

[ErikMebo]

Thaks for that! Exactly what I needed. (Well, I still have to put it into practice, but I assume it will work.)

[ErikMebo]

Hi Johnsonshiue,

I tried that, but when I project the slots to the new scetch on the square beam, it projects the slots, with both upper and under centerpoints of the slot ends, but NOT the centerpoint of the slot. Which is the point I need....

Either I am still doing something wrong, or I misunderstand your explanation.

Thanks for the effort.

[ErikMebo]

So now it does follow the update when I  SHORTEN the slotplate. But it doesn't when I LENGTHEN it. And I can't fuguere it out...

If I wasn't bald already, I would now be pulling my hairs out!

Any idea's? Anyone?

[johnsonshiue]

Hi! I guess this may have something to do with increment or decrement. The pattern may not be aware of the newly added holes. Please share the files here. I would like to understand the behavior better.

Many thanks!

[ErikMebo]

Hi Johnsonshiue, 

Thanks for that reply. In the attachment a zip file of that test assembly.

Yes I agree, it is not aware of the new holes. Question is: How do I MAKE them aware? I tried, but can't figuer it out.

Dirty solution I have for now is, in the mastermodel that we use as a sourcefile for every new project, I set the standard value in the longest size we make that in (900mm). Then if we start a new project with "Ilogic copy design" it automatically has the highest number of holes, and then we reduce it to the correct length and consequently the number of holes it needs. But if for any reason during the project it is decided to raise that number, then we have to manually add those extra holes. That doesn't kill us, but it kind of surpases the idea of automating it in the first place... I want it "Idiotproof and usable when drunk".

Thanks for in vesting your time to help us solve this!

Erik

[johnsonshiue]

Hi! I am not seeing the holes at all. Which part should I look at? tzstplaat.ipt? Please clarify.

Many thanks!

[ErikMebo]

Hi,

Yes, the holes should be in tzstplaat.ipt folowing the hole patern of slotstrip.ipt.

In the attachment you see two screenshots: One showing the right hole position, and one that's not following the adapted patern.

In the screenshhot  named "projection" you see that it does project the upper and bottom centerhole of the slot. But NOT the centerpoint. 

Thanks for trying to help!

[SBix26]

This would be so much simpler and so much more robust if you could model these in a master model as two separate but interdependent solid bodies.  Then Make Components (or manually derive them) into two separate parts.  With feature patterns using the same parameters they cannot fail.

Cross-part projections into sketches are nothing but trouble, especially when patterns are involved.  If you can't use the master model technique, then I think your current parts will work much better if you link the pattern parameters (qty and spacing) from one part to the other instead of trying to force projected sketch geometry to make feature patterns.

If I get time in the near future, I'll try to provide you an example of each method.

---

Sam B

Inventor Pro 2025.2 | Windows 11 Home 23H2

[johnsonshiue]

Hi Erik,

I am not familiar with your model. If possible, please share the files in a state that can easily reproduce the behavior. I am sorry I have limited bandwidth guessing how to reproduce the behavior.

Many thanks!

[ErikMebo]

Hi Johsonshiue,

I have shared all files two messages ago in a zip file as a pack & go. Can you open these? Or not? I attached them again here.

[ErikMebo]

Hi SB XI 26,

That sounds very interesting. And I'm glad to hear there is a better option than cross part projections. Now linking the parameters and references of two parts I'm familiar with. But how do I get the coordinates of the starting point od that array acrros?

I've heard about the concept of a master model technique. And tried to find manuals or instructions about it but failed. Can you point out where I can find an elaborate explanation or manual on that subject? 

Looking forward to your examples and thanks for your effort!

[SBix26 · Accepted solution]

Here is your assembly using the master modeling method.  [I realize that most of the model you shared was quickly constructed for this topic in the forum, but I'm struck by how underconstrained some of the parts are.  Sketches without reference to the origin, nominal measurements but without dimensions-- don't do that!  Make sure all sketches are fully constrained!].

In any case, the master model part (shown below) controls the geometry.  It contains five solid bodies, individually colored for easy identification, and you can see in the model browser that there are five features that are labeled "New Solid".  The five individual component part files are derived from those five solid bodies and are then placed into the assembly and grounded-- no constraints required unless there is movement in the assembly.  To make changes, edit as needed in the master model file, then click the Update button in the assembly.  That's it.

The attached assembly is Inventor 2025 format.

---

Sam B

Inventor Pro 2025.2 | Windows 11 Home 23H2

[ErikMebo]

Hi SBix26,

Now THAT'S an elaborate reply. THANK'S for that! And I gladly accept the rebuke about the lack of constraints in the sketches. You are completely correct in your assumption that I gobbled this up for this forum. 

Solution accepted.

Have a nice day.

Erik

[johnsonshiue]

Hi Erik,

I did see the files and I also took a look. The problem is I don't know exactly what you did to create the holes. If possible, please share the parts that already contain the holes. Then I can try mimicking your workflow to see the failure.

Many thanks!

[ErikMebo]

Hi,

Ok. Thanks for that. Before you go on, I did receive a solution to the problem. So it's up to you if you still want to invest time in it.

Here's a step by step explanation.

Put a point in a sketch on the front of a sheetmetal.

Name it's constraints. (I think it was offset.)

Put a slot on it. (with a centrepoint slot command!!!)

Add a rectangual patern to it.

Defined the number of slots and spacing with a formula to define the SPACING and NUMBER of slots, depending on the LENGTH of the strip. 

Named these parameters.

Imported this part into the assembly.

Constrained it in all directions.

Shared the slothole sketch.

Put the tzstplaat in edit mode

Projected the slotplate's sketch on it. (This is the point where I can NOT select the centerpoint of the slot so I have to call for the initial parameters of the centerpoint from the slot and define it's constraints to the sides of the projected slot plate. )

Then I add the hole's in the tzstplate.

I aded a form to the slotplate ipt in Ilogic to define the length of the slotplate. 

If I then LENGTHEN the slotplat, it atomatically adjusts the length and the number of slots in theslot plate IPT. But NOT in the Tzstplate ipt.  If I shorten it, It all folows.

The solution I found is redefining the hole's in the tzstplate with the same parameters I had for the slot definition in the slotplate ipt. But projecting them was clearly not a workflow that did the trick.

I hope this clarifies the corrupted workflow I used. I just could not get my head around the fact that projecting geometry is not functioning as good as I was expecting. Apparently you really need to completely redfine the hole positon and parameters on the new part if you want them to correspond with the position of the slots. Counterintuitive if you ask me. And it defies the whole concept of adaptivity if you ask me. But hey, I'm just an aspiring designer. Not a vetted one yet...

Cheers!