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Drawings Stamp with Date

18 REPLIES 18
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Message 1 of 19
BDUB2012
4608 Views, 18 Replies

Drawings Stamp with Date

Currently in autocad we start the print/plot command and then the command line shows options for the drawing stamp. There are several options including for approval, approved for construction, test only and others. When the appropriate number associated with the correct drawing stamp it lets you pick an insertion point and inserts the drawing stamp with a curretn date under the stamp to show when the drawing was plotted. After the drawing stamp is inserted it returns to the print/plot dialog.

 

If any IV users have a simular drawing stamp with date that is put on their drawings, I would like to hear how it was accomplished.

 

I have played with a sketched symbol and with ilogic can insert the symbol and start the print/plot command but I do not know how to make the stamp selection in ilogic automatic with a parameter or ipropery.

 

If ilogic is the way to go with this please reply with suggestions and it not please reply with other options to accomplish the drawing stamp insertions with current date.

 

Thanks

18 REPLIES 18
Message 2 of 19
yannick3
in reply to: BDUB2012

Hi

see this link

http://beinginventive.typepad.com/being-inventive/2011/07/plot-date-stamp-in-title-block.html

 

Yannick Verreault
INV PRO 2015
MS Office 2007
Win 7 pro, core i7 950, asus P6T WS
nvidia Gforce GTX 295
WD caviar black 500Go
WD caviar black 1To

Message 3 of 19
BDUB2012
in reply to: BDUB2012

That looks like it would work well but in my case I kind of pictured have several sketch symbols (one for each stamp option), then somewhere have a parameter or ipropery that you select or enter the stamp needed and when an ilogic rule was ran it would look to see whcih stamp was selected and insert that stamp in a specified location on the drawing and update the date that is under the stamp and then initiate the plot command.

Message 4 of 19
nmunro
in reply to: BDUB2012

A more comprehensive solution is available.

 

http://www.c3mcad.com/ProductPages/Drawing/ProductPlotStampPlus.aspx

 

 

 

        


https://c3mcad.com

Message 5 of 19
BDUB2012
in reply to: nmunro

The first link just dealt with the plot date stamp not how to deal with miltiple stamp selection and the second link was a purchase item and that will not be possible.

 

Is it possible with ilogic to prompt the user for input to select the stamp needed and then insert that stamp.

Message 6 of 19
SBix26
in reply to: BDUB2012

Yes, it is possible to prompt the user for input-- check out Forms in iLogic.  Combine the information in the first link with a custom form to get the function you need.  Since nobody is offering a ready-made solution for free, you will either have to learn iLogic for yourself or pay someone to for their time.

Message 7 of 19
bobvdd
in reply to: SBix26

Let me volunteer Smiley Wink

 

Attached is a sample IDW (that can be used as drawing template if you like).

Display the iLogic browser and start Form1.

It allows you to select 3 status choices.

The result is stored in the Status iProperty and in the drawing titleblock.

And the plot date of course is also introduced in the titleblock.

Capture.JPG

 

Here is the ilogic rule that uses a multi-choice parameter called "DrawingStamp"

 

Dim odrawdoc As DrawingDocument
odrawdoc = ThisApplication.ActiveDocument
customPropertySet = odrawdoc.PropertySets.Item("Inventor User Defined Properties")
Try
      prop = customPropertySet.Item("Plotdatestamp")
Catch
      customPropertySet.Add("", "Plotdatestamp")
End Try
Try
Dim PlotDate As Date
PlotDate = Now

iProperties.Value("Custom", "Plotdatestamp") = PlotDate
iProperties.Value("Status", "Status") = DrawingStamp 

Catch
End Try
InventorVb.DocumentUpdate()
Dim oCtrlDef As ControlDefinition
oCtrlDef = ThisApplication.CommandManager.ControlDefinitions.Item("AppFilePrintCmd")
oCtrlDef.Execute

 

Bob




Bob Van der Donck


Principal UX designer DMG group
Message 8 of 19
karthur1
in reply to: bobvdd

Bob,

Just got a chance to check out your drawing.  When I try to open it, it gives me an error... "The docfile has been corrupted"....

 

 

2012-04-17_2002.png

Message 9 of 19
bobvdd
in reply to: karthur1

The drawing that I attached originally is in 2013 format.

Here is a 2012 version of the drawing.

 

Bob




Bob Van der Donck


Principal UX designer DMG group
Message 10 of 19
BDUB2012
in reply to: BDUB2012

I guess I should have mentioned that I am stuck on 2011 until next year.

Message 11 of 19
karthur1
in reply to: bobvdd

I tried it in both 2012 and 2013 last night and got the same error msg in both.  The error that I usually see when its a version issue is "Error reading RSe stream".... or something like that.

 

I'll try the new file when I get to a machine with 2012. Thanks

Message 12 of 19
karthur1
in reply to: bobvdd

Bob,

Just tried to open both of your files using Inventor 2013.  Both of them give me the same error as I posted above...."The doc file has been corrupted".

Message 13 of 19
bobvdd
in reply to: karthur1

This is really bizarre. I tried with a colleague here at work and he can perfectly open the 2013 file in 2013 without any error.

 

Bob




Bob Van der Donck


Principal UX designer DMG group
Message 14 of 19
karthur1
in reply to: bobvdd

I deal with "bizarre" on a daily basis... lol

Message 15 of 19
JamieVJohnson2
in reply to: karthur1

CAD Managers,

 

I took some time to work this out for Inventor 2013.  Here are the results:

 

Create a custom property or two for your plot stamp in iProperties of the .idw.

ex:

CurrentUser (as text)

PlotDate&Time (as date)

 

Edit Border Resource and add a text where you want the 'plot stamp', be sure to constrain it to your border lines so it moves with your document sizes.

ex:

<FILENAME AND PATH>, <CurrentUser>. <PlotDate&Time>

 

<FILENAME AND PATH> exists already and can be found at

  • Type = "Properties - Drawing"
  • Property = "FILENAME AND PATH"
  • Press the Add Text Parameter button to the right.

The other two will be found under Type = "Custom Properties - Drawing"

 

Create iLogic Rule at Manage\iLogig\Add Rule

ex.

Name = "PlotStamp"

Selecting from the System functions, expand the iProperties section, then select Custom once for each property you want to set.

code:

iProperties.Value("Custom", "PlotDate&Time")= Now & " " & Time
iProperties.Value("Custom", "CurrentUser")=System.Security.Principal.WindowsIdentity.GetCurrent.Name

 Attach your rule to an event such as before save:

at Manage\iLogig\Event Triggers

Select the "Before Save Document" event, then press the Select Rules... button below, then select "Plot Stamp" rule.

 

Result:

"C\VaultWorkingFolder\TTS CAD\Inventor\Templates\04 DWG TTS.idw, Domain\jvjohnson, 1/7/2013 6:51:24 PM"

 

Save with your templates and use whenever you create a new Inventor drawing document.

 

 Perhaps someday, there be an event for 'Before Print' we can hook this into.

 

Later,

 

jvj

 

 

jvj
Message 16 of 19
karthur1
in reply to: JamieVJohnson2


@JamieVJohnson2 wrote:

....

 

 Perhaps someday, there be an event for 'Before Print' we can hook this into.

 

Later,

 

jvj

 

 


 

What you really have is a "Last Saved Date", not plot date.  They just happen to be the same with this code.

 

Message 17 of 19

@JamieVJohnson2, thanks for the post. I am running Inventor Professional 2022 and the ilogic wouldn't work for me. However, I was able to figure out how this version likes to see it, so here it is for those who need it to work in a different version. 

 

Step 1:

Create iLogic Rule at Manage\iLogic\Add Rule

ex.

Name = "PlotStamp"

Selecting from the System functions, expand the iProperties section, then select Custom once for each property you want to set.

code:

 

iProperties.Value("Custom", "PlotDate&Time") = Now & " " & Time
iProperties.Value("Custom", "CurrentUser") = ThisApplication.UserName

 

Step 2:

Enter your "User Name" at Tools\Application Options, General tab, "User name" field

 

Step 3:

Create trigger at Manage\iLogic\Event Triggers

Drag "PlotStamp" over to "Before Save Document"

 

Step 4:

Edit Title Blocks resource and add a text where you want the 'plot stamp', be sure to constrain it to your border lines so it moves with your document sizes. The variables strung together below can be rearranged to whatever order suits you.

ex:

<PlotDate&Time>, <CurrentUser>, <FILENAME AND PATH>

 

In the text window, choose the properties you just created in the "PlotStamp" rule

 

First:

  • Type = "Custom iProperties"
  • Source: "Current Drawing"
  • Property: "PlotDate&Time"
  • Press the Add Text Parameter button to the right.

Second:

  • Type = "Custom iProperties"
  • Source: "Current Drawing"
  • Property: "CurrentUser"
  • Press the Add Text Parameter button to the right.

Third:

  • Type = "Standard iProperties"
  • Source = "Current Drawing"
  • Property = "FILENAME AND PATH"
  • Press the Add Text Parameter button to the right.

Cheers!

Message 18 of 19
karthur1
in reply to: kyle.guessAQTWU

There is some other discussion here about adding/creating a plot stamp function.

 

https://forums.autodesk.com/t5/inventor-forum/plot-stamp-for-idw/td-p/11894008

 

I posted the Add-in there (message #9)that I use.  When loaded this addin will write/update the info on the idw.

 

 

Message 19 of 19
johnsonshiue
in reply to: BDUB2012

Hi Folks,

 

Here are a few more discussions.

https://forums.autodesk.com/t5/inventor-forum/date-stamps/td-p/6787315

https://forums.autodesk.com/t5/inventor-forum/inventor-title-block-date/td-p/6926662

 

Many thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer

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