Embossing many elements ?

[Xazaks]

I'm just starting my adventure with inventor, so sorry if my question is simple,

but I have no idea how to deal with this problem.

Is it possible to emboss multiple elements at once, without selecting each of them separately ?

I got over 2k elements on sketch which are needed to be embosed, it would be really pain to do it manually.

Thanks for help in advance 😄

[JDMather]

Can you attach your ipt file here (or at least a screen capture image)?

[Xazaks]

Sure, the design is in mess due to dimensioning.

I just learned to use multiple copy tool recently.

On screenshot you wouldn't probably see all things so here goes ipt file.

Thanks for interest.

[JDMather · Accepted solution]

Your part is not at the origin.

Pattern Features when possible, not sketches.

You have repeated dimensions that aren't needed.

Edit your sketch and right click and select Show All Constraints.

Zoom in on the small circles.

This is unneeded complexity.

[mcgyvr]

This ilogic code works EXCELLENT for "extruding" multiple sketched profiles.. I use it to select multiple "text" elements that I extrude .001" to represent "silkscreening" on my parts.. It can probably be modified to use emboss instead of extrude but maybe extrude will work for you also.. 

If TypeOf ThisApplication.ActiveEditObject Is Sketch Then
'Do nothing
Else
MessageBox.Show("Activate a Sketch First then Run this Rule", "ilogic")
Return
End If

Dim oPartDoc As PartDocument
oPartDoc = ThisApplication.ActiveDocument

Dim oCompDef As PartComponentDefinition
oCompDef = oPartDoc.ComponentDefinition

Dim oSketch As PlanarSketch
oSketch = ThisApplication.ActiveEditObject 

' Create a profile.
Dim oProfile As Profile
On Error Goto NoProfile
oProfile = oSketch.Profiles.AddForSolid

'get user input
oDistance = InputBox("Enter Extrude Distance", "iLogic", ".001 in")
oDirection  = InputRadioBox("Select Extrude Direction", "Up (+)", "Down (-)", True, Title := "iLogic")
oJoinOrCut  = InputRadioBox("Select Extrude Solution", "Join", "Cut", True, Title := "iLogic")

If oDirection = True Then
oDirection = kPositiveExtentDirection 
Else
oDirection = kNegativeExtentDirection
End If

If oJoinOrCut = True Then
oJoinOrCut = kJoinOperation
Else
oJoinOrCut = kCutOperation
End If

' Create an extrusion 
Dim oExtrude As ExtrudeFeature
On Error Goto NoExtrude
oExtrude = oCompDef.Features.ExtrudeFeatures.AddByDistanceExtent( _
oProfile, oDistance, oDirection, oJoinOrCut)

ThisApplication.CommandManager.ControlDefinitions.Item("FinishSketch").Execute

iLogicVb.UpdateWhenDone = True

Exit Sub

NoProfile:
MessageBox.Show("No closed profile found", "iLogic")
Return

NoExtrude:
MessageBox.Show("No extrusion created, check your inputs.", "iLogic")
Return

[swhite]

Do you mean on a single sketch with multiple items, that you want to emboss onto a single part, or items you want to emboss on multiple parts?

[Xazaks]

---

@SWhite wrote:

Do you mean on a single sketch with multiple items, that you want to emboss onto a single part, or items you want to emboss on multiple parts?

---

Single sketch with multiple elements (all the same) on single part.

JDMather advice solved problem:

---

@Anonymous wrote:

Pattern Features when possible, not sketches.

---

Thanks JDMather,

this is exacly what i needed.

I didn't know that, it was possible to copy embos.

Now everything is much easier.

Once more big thanks.