Flat pattern with a rectangle that rotates | / - \ - / | ....

[FilipeMais]

https://drive.google.com/drive/folders/1x5hRR5z5_4Kz2ReUc9Tm7HF2ztKwVDcj?usp=sharing Dear all,

I'm using Inventor 2022 and I need to draw  a pattern with around 50 rectangles with different angles. In the end, it should be mirrored to the right.

I drawn like what you can see bellow.

Are the better solutions? 

Thanks in advance 😉

Full plateDetail

[JDMather · Accepted solution]

@FilipeMais 

Can you Attach your *.ipt file here?

Pattern Features rather than sketch elements.

In any case i would not duplicate sketch dimensions (have you used Sketch Blocks).

Do you have a picture of something similar that already exists in the real world?

[BeKirra]

Yes, agree with JDMather.

Using rectangle sketch block could be a better solution in your case.

Then mirror the solid features as you have already mentioned.

Note: the specific feature "pattern" function is not available in Inventor if you are looking for it.

HTH

[IgorMir · Accepted solution]

Hi Filipe,

Technically - it is not a pattern. It is a set of individual cuts. Because of their orientation. What you are asking for is to array a set of similar cuts but to rotate every occurrence of them on a specific angle. I afraid - you are out of luck here.

The part still can be modeled. It just takes a bit of a time. But not a huge amount of it, really. Here is a part in IV2020 format.

Cheers,

Igor.

[r.burggraaff]

Olá JDMather,

Thanks for your reply.

I updated the post and inserted the link to get the part.

The part already exists in the real world, but there isn't a drawing and I don't have photos of it.

Thank you 

[cidhelp · Accepted solution]

Hi @FilipeMais ,

with iLogic you can create such pattern:

Dim oLine As SketchLine = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kSketchCurveLinearFilter, "Horizontale Skizzenlinie wählen:")
If oLine Is Nothing Then Exit Sub
Dim oSk As Sketch = oLine.Parent
Dim oTG As TransientGeometry = ThisApplication.TransientGeometry

If oLine.StartSketchPoint.Geometry.Y - oLine.EndSketchPoint.Geometry.Y > 0.001 Then
	MsgBox("Nur horizontale Linien möglich.")
	Exit Sub
End If
Dim oSPt As Point2d
If oLine.StartSketchPoint.Geometry.X > oLine.EndSketchPoint.Geometry.X Then
	oSPt = oLine.StartSketchPoint.Geometry
Else
	oSPt = oLine.EndSketchPoint.Geometry
End If

HL = InputBox("Abstand zum Mittelpunkt", "Skala_1", "1500")/10
'Dim AnzL As Integer = InputBox("Anzahl Skalenstriche", "Skala_1", "10")
AbL = InputBox("Abstand Skalenstriche", "Skala_1", "100") / 10
ReL = InputBox("Rechteck Länge", "Skala_1", "40") / 10
ReB = InputBox("Rechteck Breite", "Skala_1", "10") / 10
Dim Lg As Double = Abs(oLine.StartSketchPoint.Geometry.X - oLine.EndSketchPoint.Geometry.X)
Dim AnzL As Integer = Floor((Lg - AbL / 2)/AbL) + 1

'senkreche Hilfslinie
Dim oCPT As Point2d = oTG.CreatePoint2d(oSPt.X, oSPt.Y + HL)
Dim oSLine As SketchLine = oSk.SketchLines.AddByTwoPoints(oSPt, oCPT)

oSLine.Construction = True
Ab = AbL / 2
Dim oRPt As Point2d
Dim oColl As ObjectCollection

For i = 1 To AnzL
	oRPt = oTG.CreatePoint2d(oSPt.X-Ab , oSPt.Y)
	Wi = Atan2(HL, Ab)
	oSLine = oSk.SketchLines.AddByTwoPoints(oRPt, oCPT)
	oSLine.Construction = True
	
	oHPtL = oTG.CreatePoint2d(oRPt.X, oRPt.Y - ReL/2)
	oHPtB = oTG.CreatePoint2d(oRPt.X - ReB/2, oRPt.Y)
	oReLines = oSk.SketchLines.AddAsThreePointCenteredRectangle(oRPt, oHPtL, oHPtB)
	oColl = ThisApplication.TransientObjects.CreateObjectCollection
	For Each oSkEnt In oReLines
		oColl.Add(oSkEnt)
	Next
	
	oSk.RotateSketchObjects(oColl, oRPt, PI/2+Wi, False, True)
	
	Ab = Ab + AbL
Next

oLine.Construction = True

[JDMather]

---

@r.burggraaff wrote:

I updated the post and inserted the link to get the part.

---

Why did you not Attach the *.ipt file here as requested?

[FilipeMais]

Hi Igor,

Thanks for your reply. Even more, thank you for the file. ;.)

I thought it could exist an automatic way to do it.

Because yesterday I needed to make 50 holes, but next time could appear a model that needs more than that... :-S

Thank you.

[FilipeMais]

Thank you, cidhelp,

In one word: Spectacular!

Thanks for sharing a different way to do the job.

It is a great incentive to learn how to use iLogic.

Thank you

[FilipeMais]

Sorry... I am a beginner in the forum.

Just now i see it exist a way to share a file.

I guess it is ok now. 🙂

[IgorMir]

Hi Filipe,

Yes, if you do it on a regular basis - iLogic is a great help, as had been already demonstrated by cidhelp.
Cheers,

Igor.

---

@FilipeMais wrote:

Hi Igor,

Thanks for your reply. Even more, thank you for the file. ;.)

I thought it could exist an automatic way to do it.

Because yesterday I needed to make 50 holes, but next time could appear a model that needs more than that... :-S

Thank you.

---

[JDMather]

@FilipeMais 

Where are you going with this design?

Do you have a picture of something similar from the real world in finished form?

I suspect that there might be a much easier technique if you are going where I think you are going with the final form design.