topic Re: Same dimensions not always used to define geometry - delete dimensions with in Inventor Forum

Same dimensions not always used to define geometry - delete dimensions with iLog

Anonymous — Wed, 28 Dec 2016 19:41:49 GMT

Hello All,

I am drawing a fairly simple counter-top destined for a CNC machine. I am trying to write a program so that people that don't know inventor can create a part from some basic inputs in an excel file.

Often times I do not get the same dimensions from a company to define exactly what they want - therefore I can't write a program that is failproof currently.

Inputting the parameters is fine, but I want to know if there is a way to make parameters "optional?"

Say if they enter a 0 as a radius, it would simply delete the dimension so that a different dimension could be used to constrain the sketch.

I do not know syntax to use iLogic very well but (unless there is a better command) I would want it to do something like this:

Read dimension from excel file

if dimension ==0

delete dimension

end

Re: Same dimensions not always used to define geometry - delete dimensions with

Curtis_W — Wed, 28 Dec 2016 20:41:59 GMT

Hi jrsalmon24,

More commonly we would create multiple "optional" features and suppress them.

For instance if there is not a radius then we would suppress a fillet feature, rather than a sketch dimension.

See the attached Inventor 2015 file for quick iLogic example.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Betreff: Same dimensions not always used to define geometry - delete dimensions

Sofia.Xanthopoulou — Fri, 30 Dec 2016 10:59:27 GMT

Hi @Anonymous,

I am not the iLogic expert here, too, but just trying to use common sense... For starters, Curtis_Waguespack's sounds reasonable.

To understand your needs, do you want the feature to disappear when entering "0" or do you want the entry to be replaced by another number?

And do you want to use iLogic or just using Excel to import the parameters? I am pretty sure Excel is able to handle constraints (if 0 then....)

You may consider using the Excel in combination with iParts.

Regards

Betreff: Same dimensions not always used to define geometry - delete dimensions

Anonymous — Fri, 30 Dec 2016 14:41:30 GMT

Thanks to both of you for the response, but that's not exactly what I'm looking for. When entering a zero I do not want the feature to disappear, as it is just a single dimension of the feature I am trying to create. I suppose I want it to be replaced by another number, but one that inventor comes up with, not that I have to input. I will try to explain better with these pictures, hopefully they are clear enough - sometimes I receive the dimensions such as the angle, the short length and the inner and outer radii. This works fine and properly constrains the sketch, however sometimes they will give me a dimension such as the 'total height' instead. I want to be able to enter a zero for 'long length' and the program does not use that dimension to constrain the sketch. Is that making more sense?

Thanks for the help.

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Curtis_W — Fri, 30 Dec 2016 17:33:14 GMT

Hi jrsalmon24,

It sounds like you want to change the dimension from driving to driven then?

Here's a basic iLogic that demonstrates the syntax. I would create some true/false parameters to use as toggle. In this example the true/false parameter is called oDriveLength

I'll try to provide a simple example using an iLogic form next week if I can remember.

'get the sketch to work with
oSketch = ThisDoc.Document.ComponentDefinition.Sketches.Item("Sketch1")

If oDriveLength = True Then
oSketch.DimensionConstraints.Item(d0).Driven = True 
Else
oSketch.DimensionConstraints.Item(d0).Driven = False
End If

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Betreff: Same dimensions not always used to define geometry - delete dimensions

Anonymous — Fri, 30 Dec 2016 18:28:28 GMT

Thank you Curtis.

Best,

James