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Cutting Text

26 REPLIES 26
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Message 1 of 27
AxisMC
6327 Views, 26 Replies

Cutting Text

I need to have text, laser cut out of a sheet metal part. How can I introduce text onto a sketch that IV11 can recognize as a consumable for cutting on the part without having to redraw each letter myself ?
26 REPLIES 26
Message 2 of 27
Anonymous
in reply to: AxisMC

il giorno 09/06/2006 8.16 AxisMC ha scritto:
> I need to have text, laser cut out of a sheet metal part. How can
> I introduce text onto a sketch that IV11 can recognize as a consumable
> for cutting on the part without having to redraw each letter myself ?

You can download the addin "3DText" from
http://www.cbliss.com/inventor/iCode/index.htm. It lets you create a
sketck from a text, to be used for extruding or cutting.

M.
Message 3 of 27
Anonymous
in reply to: AxisMC

But of course it will not keep the middle of the ABDOPQR, so you will
have to add tabs for these letters

MarcoA wrote:
> il giorno 09/06/2006 8.16 AxisMC ha scritto:
>> I need to have text, laser cut out of a sheet metal part. How can
>> I introduce text onto a sketch that IV11 can recognize as a consumable
>> for cutting on the part without having to redraw each letter myself ?
>
> You can download the addin "3DText" from
> http://www.cbliss.com/inventor/iCode/index.htm. It lets you create a
> sketck from a text, to be used for extruding or cutting.
>
> M.
Message 4 of 27
Anonymous
in reply to: AxisMC

unless you wanted just the letters, in which case you would have to add tabs to the lowercase i and j
Message 5 of 27
pcunningham1
in reply to: AxisMC

In IV10 you can simply add text to the sketch and extrude it. Can you not do this in 11?

-Paul Cunningham
Paul Cunningham
IV2008
Message 6 of 27
Anonymous
in reply to: AxisMC

If it was only that easy...once you extrude that text it usually has
splines in it which cannot be used for laser cutting (at least not for
ours) This means you end up redrawing it anyways.

pcunningham1 wrote:
> In IV10 you can simply add text to the sketch and extrude it. Can you not do this in 11?
>
> -Paul Cunningham
Message 7 of 27
pcunningham1
in reply to: AxisMC

Just to test, I extrude-cut a script font. It seems to break the curves down into straight line segments - see attached. (Does IV even know what a spline is?)
Paul Cunningham
IV2008
Message 8 of 27
SemiCatS
in reply to: AxisMC

FYI... ALL my round/circular sections of both normal parts and sheet-metal parts have straight segments like that. I always thought it was the graphics board that didn't do its job? I really DO miss a "regen"-command-type-thing in Inventor - just like we do in AutoCAD.
It's really annoying when you zoom into a detail to see if it looks alright, and if there's enough clearance... and all you see is a couple of straight line segments where it's supposed to be a smooth curved line/surface.

Stig M. Thu
Message 9 of 27
Anonymous
in reply to: AxisMC

Try saving as a dwg.

Plus even if they were lines, all those extra lines you put into a part
when you laser is money out of your pocket as the laser will stop at
each point for a split second, the more lines, the more split seconds.
When you can make 30 lines into 1 arc, it can make the cutting process
much shorter.

pcunningham1 wrote:
> Just to test, I extrude-cut a script font. It seems to break the curves down into straight line segments - see attached. (Does IV even know what a spline is?)
>
>
> ------------------------------------------------------------------------
>
Message 10 of 27
pcunningham1
in reply to: AxisMC

In this case, each apparently straight element is in fact a line segment, as evidenced by the highlighting of the edge in my previous attachment.
Paul Cunningham
IV2008
Message 11 of 27
pcunningham1
in reply to: AxisMC

Output to Acad = lots of line segments.
The original post made no mention of a preference for arcs over line segments, or splines for that matter. I'm not in the laser cutting business, but if it were really a cost issue, I'm sure the laser programmer could smooth out the cutting path.
Paul Cunningham
IV2008
Message 12 of 27
Anonymous
in reply to: AxisMC

Output to Autocad = lots of lines AND splines.

"...I'm sure the laser programmer could smooth out the cutting path."

You sound a lot like how the house builders talk

The foundation people screw up and the foundation is out 1" on one side
of the house. The concrete guys say "oh the framer can fix it", then the
framer gets there and says oh the drywallers can fix it, then the
drywallers get there and say the mudder can fix it, then the mudder gets
there and says the painter can fix it....and problem keeps getting
pushed down the line

pcunningham1 wrote:
> Output to Acad = lots of line segments.
> The original post made no mention of a preference for arcs over line segments, or splines for that matter. I'm not in the laser cutting business, but if it were really a cost issue, I'm sure the laser programmer could smooth out the cutting path.
Message 13 of 27
rblawson
in reply to: AxisMC

This is true only for older-generation CAM software. newer controller software is able to adjust the speed to be much more efficient wrt polylines and stuff like that.

you may, however, have a problem with file sizes.

-barrett
Message 14 of 27
rblawson
in reply to: AxisMC

Axis,

this is a problem that I have recently tackled.

when i got to my current seat, the company's workflow was to c/p standard letters/numbers from a .ipt file that was just a couple of sketches. slow & painful.

I used the 3dtext add in on Charles' site for a bit. its ok, allows for pretty precise placement of text, and it creates the text as sketch geometry. you will have to remove interior loops.

then I started using sketch text to insert the text I want. it's a little harder to accurately place the text than with 3dtext, but it's faster. In order to get this to work, we had to create a custom font with no curves and no interior loops and use that for the sketch text.

to make the font, we used a font creator software found with google and edited sth like tahoma to get to where we wanted.

some observations:
1) using "save copy as" from flat pattern in sheet metal mode gave us larger file sizes than if we used an addin called "export geometry for flat pattern" at the bottom of kent's site:
http://www.kwikmcad.com/icode/addins.asp this addin allows you to save a flat face to dwg or dxf by right clicking.

1a) the planar geometry addin works for us because what we're getting lasered never has bendlines. if you needed a flattened pattern, well: **edit** in fact it looks like bendlines interfere with the add-in.

2) you cannot change the default sketch text font. We named our custom font Tahoma2 so it would at least be a click away.

3) in terms of file size: custom font < 3dtext < sketch text. annnd export planar add-in < save-flat ~= save-as-dxf from idw.

btw, im on IV10 sp3, apparently you can RMB to export a face in 11.

HTH

-barrett

Message was edited by: rblawson (added part 1a) Message was edited by: rblawson (fixed part 1a after testing)
Message 15 of 27
pcunningham1
in reply to: AxisMC

Obviously, it's the excavators fault for not checking the trenches with a micrometer. What ev.
Paul Cunningham
IV2008
Message 16 of 27
Josh_Petitt
in reply to: AxisMC

use mechanical desktop and the text explode option in Express Tools. import the sketch into IV
Message 17 of 27
Anonymous
in reply to: AxisMC

I'm hesitant to post this in case it doesn't live up to expectations but
hopefully it works good enough to help some of you. Below is the source
code for a small VBA macro that creates a sketch that represents a text box.
It's somewhat the equivalent of a text explode.

The macro doesn't do anything you couldn't do interactively but it just
automates the process. It creates an extrusion using the selected sketch
(which should contain the desired text), creates a new sketch on the same
face as the original sketch, and projects all of the edges of the new
extrusion onto the new sketch, and finally deletes the extrusion.

Obviously the resulting sketch won't be associative to anything and will
need to be recreated if you want to edit the text.

I just threw this together when I saw this thread on the newsgroup and did
minimal testing so make sure to save your document before using. 🙂

Public Sub ExplodeText()
Dim oDoc As PartDocument
Set oDoc = ThisApplication.ActiveDocument

On Error Resume Next
Dim oSketch As PlanarSketch
Set oSketch = oDoc.SelectSet.Item(1)
If Err Then
MsgBox "A sketch must be selected when running this macro."
Exit Sub
End If

On Error GoTo ErrorFound

Dim oTransMgr As TransactionManager
Set oTransMgr = ThisApplication.TransactionManager
Dim oTrans As Transaction
Set oTrans = oTransMgr.StartTransaction(oDoc, "Explode Text")

oSketch.SetEndOfPart True
Dim oSketchEnt As Face
Set oSketchEnt = oSketch.PlanarEntity
Dim lKeyContext As Long
lKeyContext = oDoc.ReferenceKeyManager.CreateKeyContext
Dim abtSketchFaceRefKey() As Byte
Call oSketchEnt.GetReferenceKey(abtSketchFaceRefKey, lKeyContext)
Call oDoc.ComponentDefinition.SetEndOfPartToTopOrBottom(False)

Dim oProfile As Profile
Set oProfile = oSketch.Profiles.AddForSolid

Dim oExtrudeFeatures As ExtrudeFeatures
Set oExtrudeFeatures = oDoc.ComponentDefinition.Features.ExtrudeFeatures
Dim oExtrude As ExtrudeFeature
Set oExtrude = oExtrudeFeatures.AddByDistanceExtent(oProfile, 0.1, _
kPositiveExtentDirection,
kJoinOperation)

Dim oResult As Object
Set oResult = oDoc.ReferenceKeyManager.BindKeyToObject( _
abtSketchFaceRefKey, lKeyContext)
If TypeOf oResult Is ObjectCollection Then
Set oSketchEnt = oResult.Item(1)
Else
Set oSketchEnt = oResult
End If

Dim oNewSketch As PlanarSketch
Set oNewSketch = oDoc.ComponentDefinition.Sketches.Add(oSketchEnt)
oNewSketch.DeferUpdates = True

Dim oFace As Face
For Each oFace In oExtrude.EndFaces
Dim oEdge As Edge
For Each oEdge In oFace.Edges
ThisApplication.StatusBarText = "Processing Text Curves..."
Dim oEnt As SketchEntity
Set oEnt = oNewSketch.AddByProjectingEntity(oEdge)
oEnt.Reference = False
Next
Next

Call oExtrude.Delete(True, False)

oNewSketch.DeferUpdates = False
oTrans.End
Exit Sub

ErrorFound:
oTrans.Abort
MsgBox "Unexpected error while exploding text."
End Sub

--
Brian Ekins
Autodesk Inventor API

wrote in message news:5201636@discussion.autodesk.com...
use mechanical desktop and the text explode option in Express Tools. import
the sketch into IV
Message 18 of 27
rblawson
in reply to: AxisMC

Brian,

I keep getting an error at line 38 (Set oResult...)

for a part I just have a rectangle extruded 1" with a sketch including a lowercase w in Tahoma. I got errors at line 30 (set oProfile) if I included a character with an internal loop and also if i made the sketch without projected edges. perhaps something im doing wrong?

-barrett Message was edited by: rblawson
Message 19 of 27
Anonymous
in reply to: AxisMC

I just tried a lowercase Tahama w and it worked for me. Any text that you
can successfully extrude should work with this program. If the Extrude
command fails on the text, then this will fail too.

In your case there must be something different than my test. If you can
post it I'll take a look.
--
Brian Ekins
Autodesk Inventor API

wrote in message news:5202858@discussion.autodesk.com...
Brian,

I keep getting an error at line 38 (Set oResult...)

for a part I just have a rectangle extruded 1" with a sketch including a
lowercase w in Tahoma. I got errors at line 30 (set oProfile) if I
included a character with an internal loop and also if i made the sketch
without projected edges. perhaps something im doing wrong?

-barrett

Message was edited by: rblawson
Message 20 of 27
rblawson
in reply to: AxisMC

not working in either 10 or 11. perhaps its something to do with how I copied in the macro, I dunno.

here's my file:

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