topic Attention Dimensions in Inventor Forum

Attention Dimensions

jmfowler1996 — Mon, 21 Aug 2017 12:56:44 GMT

I was going to post an idea in the ideas forum, but I wanted to first double check that something doesn't already exist which could solve my problem.

I want to really minimize the posibility of human error when using inventor. At the same time, I want to streamline the processes to make things as quick and simple as possible.

Using templates for different types of parts which I make regularly is a great way of reducing the time it takes to create models. The problem I have is that when you make a template, you need to input default values. This means that when you make a part using a template, it is possible (and has happened before) that I might forget to change one of the default values and end up with problems down the line. This may not sound like a big problem, but trust me; if you are rushing to get hundreds of profiles fabricated, you really don't want to find that some of them are made wrong for this reason. And sod's law it's probably the expensive ones.

Basically, I was wanting a way to make sure that every dimension has been edited/approved for each new part made from a template. I know you could go through the list of parameters one by one, but i'm sure you can understand that for models with lots of parameters, it is much more convenient to edit the dimensions from within the model, so that it is obvious what they are used for.

I was going to suggest some type of placeholder dimension type, which would bring attention to the author, that something still needs changed/approved. (which could also be handy for temporary values when making a model you don't have final dimensions of)

If something exists which could reduce the chances of something going wrong when using templates, I would really like to know about it.

Thanks.

Re: Attention Dimensions

-niels- — Mon, 21 Aug 2017 13:26:57 GMT

Couldn't it be as easy as scaling up your template's dimensions by a factor 10 (or 100), or at least the required parameters?

It might break the model in the template, but even that would help getting a visual indication of what still needs editing...?

I guess there would be some iLogic ways to check your parameters...
You could add a decimal value in your tempate, like 10,00001 and have an iLogic rule search for any of those values that haven't been changed yet.
(no idea on the exact code though, but i'm pretty sure it would be possible.)

You would either have to make sure to run the rule or make it run on save or something...

Re: Attention Dimensions

mcgyvr — Mon, 21 Aug 2017 14:18:36 GMT

^^ yep.. lots of potential ways to attempt to idiot proof anything..

Usually the idiots end up surprising you though as we all know....

But yes this is very "template/company/process specific" though...

However I'm sure some sort of ilogic could do it...

Ilogic form or message boxes to prompt for all variables?

Count all dimensions, set a custom property when a dimension is updated, when the total count and updated count match alert someone,etc...

or many other ways depending on specifics..

Re: Attention Dimensions

salariua — Mon, 21 Aug 2017 14:31:31 GMT

I was going to suggest AutoLimits on area or perimeter or mass, but both @mcgyvr and @-niels- have better solutions for you.

Re: Attention Dimensions

jmfowler1996 — Mon, 21 Aug 2017 14:41:04 GMT

Thanks for the response.

I thought about using really small default values a while ago, but decided against it.

I think it was because it can be difficult to tell if an already small value is even smaller, e.g. if a hole is 5mm offset from center or 0.5mm offset from center. It might be noticeable if you are looking for it, but if not, then nothing will look out of place. I have a few other nit-picky issues with the idea too, like that infrequently, geometry can act up if parameters are vastly changed, and it would be nice to be able to insert a part into an assembly just to see how everything comes together, but still be reminded to come back to the dimensions later.

I like your idea of adding a negligible value to the dimensions and checking with iLogic. I probably will try something along those lines. Although I'm just thinking, it might cause problems with constraints if the values arent exact? Maybe not. I mean like if there was a line at 45 degrees, but dimensioned vertically, adding 0.00001 to the dimension would add about 0.0000141 to its length, which might cause constraint problems with the geometry it's in. I suppose that's highly unlikely.

What I'll do is when I get some time, I'll have a go at making some code for this. I still would have preferred an elegant built-in solution though. Especially considering how much time I spend creating parts like this. Maybe I am in a bit of a niche situation though.

Thanks again!

Re: Attention Dimensions

salariua — Mon, 21 Aug 2017 15:04:01 GMT

Boolean checks boxes for each dimension with trigger ON SAVE.

If the user has ticked the box then he has approved the dimension.

Re: Attention Dimensions

johnsonshiue — Mon, 21 Aug 2017 16:34:37 GMT

Hi Guys,

We have customers using MBD/3DA workflows for dimension checking purpose on Inventor 2018. The nice thing about MBD/3DA is that the dimension values are bounded to the geometry, not to a feature or something. This can help check critical dimension without having to go through parameters table.

Many thanks!

Re: Attention Dimensions

jmfowler1996 — Thu, 24 Aug 2017 12:07:10 GMT

Okay, so this is what I ended up doing:

Create a user parameter named "Check" (=1ul)
For parameters which require approval/changing, divide their expressions by the "Check" parameter (e.g. d0 = 10mm / Check)
Run a rule to find any parameters with the string "Check" in their expression and prompt for the value to be approved/changed.
Have the rule run on save.

The main advantage of this method is that it is possible for the user to go into the part and edit the parameters within the sketches/features rather than in a list of parameters. Thanks to niels who gave me the idea.

Here's the code:

oDoc = ThisApplication.ActiveDocument
Dim uom as UnitsOfMeasure = oDoc.UnitsOfMeasure
For Each oPar In oDoc.ComponentDefinition.Parameters
If InStr(oPar.Expression, "Check") Then
If uom.CompatibleUnits(oPar.Value, oPar.Units, "1", "mm") Then
unitType = uom.LengthUnits
defaultUnits = "cm"
ElseIf uom.CompatibleUnits(oPar.Value, oPar.Units, "1", "deg") Then
unitType = uom.AngleUnits
defaultUnits = "rad"
End If
oPar.Expression = InputBox(oPar.Name & " (= " & uom.ConvertUnits(oPar.Value, defaultUnits, unitType) & ")", "iLogic", oPar.Expression)
End If
Next

As a bonus, making the "Check" parameter = 0 highlights the relevant parameters, since they are dividing by 0.

Thanks for all of your input.

Re: Attention Dimensions

salariua — Thu, 24 Aug 2017 12:28:37 GMT

@jmfowler1996 wrote:

Thanks for all of your input.

well done. I will try to remember your solution.

another possible way is to have it in Comments but the "division by 0" you mention won't work.

if comments contains "Check"

If InStr(oPar.Comment, "Check") Then

if comments starts with "Check"

If oPar.Comment.StartsWith("Check") Then

result :

Re: Attention Dimensions

-niels- — Thu, 24 Aug 2017 12:50:26 GMT

@salariua, am i correct i thinking that if you put "check" in the comments it will keep checking the value until the comment is cleared?

If so, @jmfowler1996 solution of putting it as a parameter would be the better option as that would be easier to replace when editing a sketch...

Still, with iLogic you could probably make a box with all the required parameters listed and then have it clear the comment when the value is changed...

Re: Attention Dimensions

salariua — Thu, 24 Aug 2017 12:58:56 GMT

@-niels- wrote:

@salariua, am i correct i thinking that if you put "check" in the comments it will keep checking the value until the comment is cleared?

True... I lost track of the requirements along the way...

my bad,

ALL, ignore my previous post.