Embedding Parameters into Template!?!?!

[Anonymous]

Folks,

I have of late been updating our drawing process in inventor. The aim is to have as much embedded info within the .ipt template that just needs to be filled out or "chosen" with a simple mouse click or minimal manual typing. All this is to minimise manual error in the Parts list when it comes to generating the drawing (general typos etc).

Now I am almost where I want to be but there is still room for error that I would like to eliminate.

My template has various custom iproperties linked to parameters to suit specific types of steel, for example if I had a bit of SHS I would insert my custom iproperty =<SHS> into the description field, which would produce the following formula:

SHS <HEIGHT>x<WIDTH>x<THK> - <LENGTH> LG.

In my template, I also have a list of parameters which are:

HEIGHT

WIDTH

THK

LENGTH

DIAMETER

To get the formula to work you have to link the appropriate dimensions to the correct parameters. This means that once you have modelled your part, you have to go into the parameters and click on the "HEIGHT" parameter  and link the equation to the appropriate dimesion, which means typing in d0 or d1 or d2 etc.

Now this is where mistakes can be made as you could link the "THK" parameter to the dimension that is actually the length (there is a chance of this happening if the dimension numbers get to d101 and d110 etc).

What I would like is a way to just click on the "HEIGHT" parameter and then somehow just click on the dimension. This would save manually typing the dimension name.

Is this possible? Or is there a slicker way to go around this?

All help is greatly appreciated.

Thanks

p.s. You guys may notice that I will be posting loads of these types of messages as I try to smooth out our drawing process. 😉

[mflayler2]

Why not just use List Parameters while you are modeling?  Make that part of the process.

[Anonymous]

forgive me if I've misunderstood or missed something. . .

But can you just create the extruded shape in the template, and have the model all set up to start with?

We do this here with a number of common components. We just start a new file using the template with the 3D part alreay created in it, and then edit a couple of key features (change length, hole sizes, etc). It's kind of like iParts but without the overhead.

Just a thought.

[Anonymous]

Cant use List parameters as the dimensions of the parameters are determined by a master sketch (we use skeletal modelling), so the dimesnions cannot be input via the parameter box.

If the master sketch changes at all, the component will change to suit and I need the parameters to change to suit also.

Thanks

[mflayler2]

So...

If you are designing your Master Sketch and you already have parameters placed in the Parameters box (HT, W, L, etc) then as you designing your Master Sketch you use the List Parameters to call forth the value in the Parameters box.  Why is that a problem.  As I showed in my graphic above if you are trying to tie a dimension to a user parameter you just have to grab it from that List Parameters box.

My understanding of your post is that once your part is modeled you go back and link HEIGHT to d0 or d1, which is exactly what List Parameters will do.  It will link HEIGHT to d0 as you are dimensioning it so there is no need to open the box up and then assign it after the fact.

Now if I am mistaken with what you are trying to do, you could still at the dimension line type in a more specfic name for the dimension so that it does not read d0.  Simply type HEIGHTPM = 2.673 and then you can link it much easier to HEIGHT after the fact.  I just don't see why my method wouldn't work for you.

[Anonymous]

Sorry, Im maybe not just making things clear.

If I was to use values within the parameters box then these values would become static. They need to be flexible i.e. when I start up my template the HEIGHT parameter is at 1mm (as default) now if I sketch something and go to add in the dimension and click list parameters and choose HEIGHT, it will make this dimension 1mm. The only way I can change that is by going into the parameters box and altering that dimension.

Now if I give that same dimension a value of 100 THEN go into the parameters box the HEIGHT will still be at 1mm but there will be a dimension called d0 and that value will be the 100 that I typed, so if I put d0 into the HEIGHT parameter equation box then the HEIGHT parameter becomes flexible. I can change the value of this parameter just by using the edit sketch or the edit feature. There is no need for me to go into the parameter box again.

BUT, as I said in my earlier post, I want a way to eliminate typing in the dimension name (d0) into the HEIGHT parameter box, I need a more slicker way of doing it.

Thanks again

[mflayler2]

So how about the designer applying a more descrete name during the inital dimensioning process and then linking it that one time?

Or perhaps if you are using iLogic you could create a Trigger to do some of this for you or maybe a simple configurator that would create the values.  If your designs are always very similar this would be a good way to go or a simple start part like BMiller said.

I guess the big question is how different are the designs from one iteration to another?

[Anonymous]

You can still use Mark's method.  Even if you don't know the exact heigth you need upon opening the template, before you start cketching beyond what is there when you first open the new part, go directly to the paramters box first, type in your values, update the sketch and then start modeling away.

If I use a template with set paramters, when I open that part, I don't draw a single line until all of the known values (or estimates of said values) are inputed into the paamters dialogue.  This eliminate the confusion of mixing up pertinent values.

Actually what I have done is created a part with an embedded spreadsheet which contains paramters for several parts that are contained in a top level assy which I call the calculator.  Since the part models will be working in conjunction with each other, I use my paramters to control several parts at once where features are going to line up or at least be relative to each other.  Then, when I link the "calculator" part to the others, all of the main driving parameters are already present, and then I model whatever else is needed on the individual parts from there.

I guess my best example would be when I create a new fridge.  I have at least 12 parts that always connect, and certain features on those parts that are driven by each other.  My primary driving dimensions are the fridge heigth, width, and depth.  I base all of my other paramters from these three numbers.  All 12 of these parts have templates that are linked to my calculator.  I open my calculator first, and type in the three numbers.  Then I start opening the template parts.  Thay are already set up to reference the calcutor and therefore the only thing I need to add is any custom features that will be relevant to the new design.

Hope that helps or least gives a little insight.

[Anonymous]

It seems like what you want is parameters that can be filled out that will already exist when you start a new part. When you create your template you can define user parameters without creating any sketch or part. If you open the parameters dialog from the manage tab the select "add numeric" in Inventor  2011 or I believe it is just add parameter in earlier versions then it will add a line to give the parameter a name.

Once you start a new part with the template these parameters will be in the parameter dialog for that part. There you can add the dimensions for the specifc part. in the dimensions, instead of typing the size, the designers can type the parameter name. this will keep everything tied to the prenamed parameters.

I would advise keeping the names as short as possible to reduce the amount of typing needed.