Positioning features with parameter

[Anonymous]

Hello,

I'm fairly new to inventor, and have a problem/question. (so please keep answers understandable for newbie)

I want to be able to position certain features of my part on a relative distance to the (0,0) centerpoint using parameters, so that I can easily adapt the part when placing it in in assembly with "place iLocig component". This works just fine for positive coordinates, but when i want to place the feature below or left the center point ( type e.g. -5 in the parameter dialog box) inventor just ignores the minus.

I position the feature with the "dimension" button in sketch. I believe inventor ignores the minus because a dimension cant be negative.

Can anyone solve this without moving the centerpoint from its original position?

[JDMather]

Attach your file here.

[Anonymous]

thanks for your quick response!

here's the file. (thing is in dutch, sorry for that)

when you open the paramater dialog box, play with the X_shift_hartlijn value. typing 100 gives the same result as -100.

[JDMather]

It sounds to me like you are trying to position a part in an assembly by changing the position of the part by the part's coordinate system within the part. 
If so, I don't think this is the way to do it (although I'm not entirely sure what you are doing).
I would use assembly constraints.

[Anonymous]

I have no problem with the assembly.

The case: my company uses a standard part rather often, but always with different geometry. I'm trying to create a standard part, that using "place iLocig component" can easily be adapted by changing the parameters.

About the attached (sheetmetal) part: I've created a loft from a rectangle to a circle. The position of the circle isn't fixed, and differs almost every time we use the part. Therefore I tried to position the circle by using simple geometry from the (projected) center point to the circle midpoint. I want the position of the circle to be controlled by parameters, using a standard XY coordinate system. This works fine for positive coordinates, but when I enter a negative parameter, thus a negative dimension, inventor ignores the minus. In other words, the circle is "stuck" in one quadrant. When I enter a negative value I need the circle to "jump" over the axis.

hope this clarifies the situation.

[Anonymous · Accepted solution]

Offhand I would suggest making a larger 'fake' quadrant. Instead of basing your center location off of 0,0 make a line that is offset by a number that is larger than the greatest positional change.

You can do this by creating a point that is offset as described from the center both in the x- and y- directions. Then in dimensioning the location of your lofting circle you base these off of the 'offset point' with the parameter for the x direction being (distance offset + positional distance) which when the positional distance is set at 0 will put your part at 0, when set at negative it will move the part to the left up to the distance that you put in for offsetting your base part. That would be the simplest way.

In order to add some intelligence/adaptability to the part I would suggest the following.

Where the Parameter 'X' and 'Y' is driven by iLogic

Base Point Distance from Centerpoint [Negative/Left Direction] {BP.X} = abs(X) * 1.1 ul

Base Point Distance from Centerpoint [Negative/Down Direction] {BP.Y} = abs(Y) * 1.1 ul

Circle Centerpoint Horizontal Distance from Base Point [Positive/Right Direction] = BP.X + X

Circle Centerpoint Vertical Distance from Base Point [Positive/Up Direction] = BP.Y + Y

Please note that the 1.1 can be changed to anything greater than or even equal to 1. This is all assuming that the value in a User Parameter will still read as positive through the iLogic function.

Edit:

See Attached Part: Note I didn't add comments as they are all included in this post and should be self explanatory.

[Anonymous]

Thank you, I can work with this.