Family Table and Parameter Column

[TomD.inPDX]

This question is to confirm something with regard to Connection Parameters used in Family Tables.

When you you use mechanism connections, in my case the General Constraint set, I found an odd behavior.

I have a part in an assembly with X-Y translations limits. I also enabled the zero position.

In Family Tables, you can access connection parameters and I set TRANSLATIONn_ZERO_POSITION in the table for X and Y.

What is weird, and what I want to confirm, why is the value set in the Family Table additive rather than value used in the position?

Here is a better explanation: I have a range from -5 to .5 assigned to my X position. My zero position is .5. But when I assign -.5 in the table, it becomes additive and offsets the mating planes in the instance. In fact, the only way to make this work correctly is to use 0 and 1 for the range I have specified.

Is this normal or have others found issues with this?

Here the 1st image is the generic: Notice how the ,measurement comes from the center of the lower hole. The regen value is .5

...Now the instance with the value set at 0.5

...notice how the start of the offset moved 1" and then the -.5 from the family table is applied.

Is this expected behavior or a bug?

Creo 2.0 M040

I was hoping to test this on M070 but it is late in releasing.

I have attached the file for testing.

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[BrentDrysdale]

Hi Tom,

Have not read this in much detail but the negative value in a family table is something that caught my eye. I have had difficulties with this before (way back) and like you have moved to an "always positive" way of dealing with it.

From memory I made a Relation with a Variable that gave a range that could be used in Family tables as always positive. e.g. ROTATION_ANGLE = d1+90 for an angle (d1) that varied between +/-90. You have to mess around with the syntax to get everything working correctly but this is the general thrust of it.

Sounds like this is simply confirming what you experienced.

Regards, Brent

[TomD.inPDX]

Thanks Brent. Very good input. I guess I'm missing the logic of how Creo is dealing with these variables.

[BrentDrysdale]

Hi Tom,

I think the logic is that PTC dropped the ball in the FT functionality to be able to handle variables that could be come negative. Pity as the models can deal with it and I ended up simply adding this extra layer of stuff on top to deal with the shortcoming. Maybe somebody figured out something else but seems like it is still working just like it always did so I would not expect any change in behavior in any upcoming release.

I did sometimes think about the way in which I dimensioned something in a model to overcome this issue and that was an alternative to making a relation though I usually ended up making a relation to more sensibly control the working size/dimension. For example instead of dimensioning an angle so that it can go between -90 and +90 through zero I dimensioned it another 90degrees further around so that it went between zero and 180 however these types of dimensions are always unintuitive later on even when I went back into my own model and this is what I would usually write a relation and control with a parameter so at least it was documented.

Now I just have to get my Creo 2 working again as something has changed that has stopped it. Not enjoying Windoze 8.

Regards, Brent

[TomD.inPDX]

I just found one option that really messed it up. Somehow I stumbled on the best way to deal with the problem.

I am switching the parameter ...ZERO_POSITION which seems to be an offset from the -picked- zero. This is -not- the value set by position, which in this is case is actually d2.

Now d2 cannot be picked as a FT "dimension" column... it has to be -entered- in "other". But when you enter a negative value for d2, a warning comes up about a "toggle" issue with things going negative each time you regen. Sure enough, when I give d2 a -.5 value, and I open the instance, it never has a successful regeneration. It just toggles back and forth between .5 and -.5 where the -minus- in this case just mean "opposite" not necessarily a real value.

Yep, this is hokey in every sense of the word.

This "toggling" effect is not true for the ZERO_POSITION value and no message appears when you do this.

So now I have a little better idea of what the ZERO_POSITION value really is (it's the Set Zero Position in the constraint dialog), and therefore it really is what I suspected, an offset from the parent relation.

But you are right, Brent. The actual dimension (.5 in my images) is an "other" column in the FT. And they do warn you to avoid negative numbers in this case. This is likely why they have the Set Zero Position option in the constraint dialog.

But why I have to go to information to find the dimensions related to the connection feature is yet another example of archaic this interface is. I should be able to pick Dimension in the FT column and select the connection feature and have the dimensions show up. But -noooo-, you have to learn what "other" means

Okay, I got that out and I'm happier with all this now.

[TomD.inPDX]

I tried creating a new copied assembly (which lost the family table, BTW) and replaced the ...ZERO_POSITION values with d2 and d3 "other" columns in the family table. I also reset the connection values to be positive at all times by entering an offset. Now I get "disconnected" errors in the regen field and the positions are completely wrong.

How do you guys live with family tables? I make a change in generic and save, and a warning that says the instances were not regenerated. I go to the family table and I don't have the option to re-verify the instances. How are you suppose to regen each instance for a successful save?

[BrentDrysdale]

Hi Tom,

Painful experience is how we live with their foibles.

Again doing this from memory as Creo not running but...

When you have your FT dialogue box open and you can see the lines of instances then in the dashboard of that box you should see a couple of icons which will give text if you hover over them. You are looking for the one that says something like "verify instances" and when you click on it it opens a sub-box that shows the instance lines and whether they are verified or not. You can choose to verify a specific instance or there is an option to verify all. The successfully verified instances say "successful" when they are done.

The method is that Creo actually regenerates the instance to check that it works and updates this sub-box with the results. For complex models with lots of regeneration this can take a while but mostly it runs OK for me. This takes care of your last question without having to open each instance to have it regenerate.

Hope this helps. Brent

[TomD.inPDX]

Right, I know that dialog: "Verify instances of the family". Problem is, it is not always accessible.

When the save warns me of non-regenerated instances, that selection is grayed out even when I have a green light on the regen indicator in the generic assembly. I have a similar problem with drawings. I can go to each instance to regenerate but who wants to do that?

When I can reproduce the problem reliably, and once I load M070... I will get with customer support on this. It is crazy not to be able to regen the instances to have a successful save.

[TomD.inPDX]

Okay, I was able to duplicate the problem.

Save notice:

Verify instance gray:

Quick video of the failure repeated: Using view states (explode) to cause the problem. This is not the only cause, however.

Video Link : 4184

Notice how repeating the save command works the second time. This is very poor behavior!

PS, all the files in the regen warning are the 3 instances in the FT's

[ptc-5008082]

Have you played with the 'Tools > Absolute / Relative Dimension Values' inside the Family Table? (highlight dimension in family table column header first) A dollar sign will be added to show that the values are to be absolute

I have not used it for connection parameters but it works with 'normal' dimensions when we want to use a negative value.

[TomD.inPDX]

That's a great tip, Charlotte! I just tested this with my selections but it is not adding a $.

This option must be very selective on what dimensions this applies to.