parametric point pattern

[ptc-4958059]

Is point pattern parametric?????????

and if it is can anyone tell me that how we can make it parametric ??????????

Give one example of it????????

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[TomD.inPDX]

Point patterns of patterned features are parametric, yes.

The sketch controls the points and if you use guide curves of surfaces, it will respond parametrically.

When you define the feature pattern, use datum points in an internal sketch (references; edit). Options gives you lots of ways to relate the pattern to other features.

Have you looked at the help files?

[ptc-4958059]

Thanks for ur kind help.

but my concern is tha for a model i have made a sketch with 24 holes on a certain PCD and now it i have to change the no of holes to 36 from a excel parameter.

is it possible by Point pattern automatically????????

[TomD.inPDX]

I am not certain I understand your application although other might understand better.

I have not used Excel files to drive part parameters.

Normally, family tables manage changing patterns for parts that define several configurations.

In family tables, you specify the parameters you wish to apply to each configuration. One may have 24 holes and the angle for the angle for the bolt circle is 360/24 where another part would have 36 holes and the angle would be 36/360.

Are you maybe asking how to update a family table using an excel file?

We can help better if we know more about your application and what you already understand.

[ptc-4958059]

thanks...

but you are not getting my point.

Point pattern is govern by a sketch in which points are placed at a certain angle with each other. rght??????

suppose that i have made a sketch with 24 holes (means 24 points) at a certain angle.

and now if i have to change it to 36 no of holes (means 36 points) with the angle changed between them,i have to modify the sketch manually rght??????

so my question is that is there any other way (except family table) that i dont even open the sketch and the no of points changes to 36 with the angle between them changed????????

please help!!!!!!

[TomD.inPDX]

There are certainly ways to do this, but without family tables, it is not logical to do so because the change would suggest a different part at any subsequent level.

However, I would not use the point table to do what you are asking. I would pattern the hole with relations that determine the number of holes based on the PCD. You could have a master hole, placed at a PCD and in relation, you would have IF statements to determine the appropriate patterning values, including number of holes.

This is a case where you are trying to use a hammer where a screwdriver is the appropriate tool.

The example logic for the for the relations IF statement would be:

if PCD = 100

instances = 24

angle = 24/360

if PCD = 120

instances = 36

angle = 36/360

else PCD = 100 (reset to a default if error entry)

These relations drive the parametric locations based on bolt circle diameter as an example.

This has nothing to do with excel files either. You have not clarified where controlling the model with excel files apply.

...I do use similar techniques on vacuum flanges. This include a large number of parameters that can size an entire flange and its features based on a single parameter. I use relations rather than family table because I find them more stable for my use. I only do this if I need to copy the file often or I need to make the change on the fly in a development effort.

[BrianMartin]

In addition to Tom's excellent reply, I wanted to add that to use patterned points in a sketch, be sure to use Geometry Points, not Construction Points. If you use a construction point, you will not be able to use it as the basis for a point pattern feature.

If you're having difficulty with point patterns, make sure you're using the right type of points!

Thanks,

-Brian

[TomD.inPDX]

Good point on the points, Brian. I always called them datum points but now I see my error after hovering on the icons

[BrianMartin]

Yeah they always were datum points until PTC removed the Axis Point option and then created the Geometry Point and the Construction Point.

Honestly I think they just confused things. It was easier to understand before. Add a point... and it shows up as a point. Add an axis point... and it shows up as an axis.

Had they allowed you to create an AXIS using a sketch even if that sketch was standalone and not tied to a feature (like a cut or protrusion), that would've been something. Instead they gave us this messy hodgepodge and most people couldn't tell you the difference between the two without looking for that table that explains them both (in the help files). Heck, most people don't know about the table! (See below).

Oh and the part in the table that says you can create an axis in a sketched curve using a datum axis is a misnomer. No one's trying to create an axis parallel to the viewing plane in a sketch (exceptionally rare). Instead, you'd like to create one normal to the viewing plane (like the old axis point function or like the new geometry point in an extrusion).

[TomD.inPDX]

(I think we're veering off topic pretty darn quick here )

[vzak]

One small additiona to the above : besides dketched points, also array of Datum Point feature can be used as a reference. Means you can create several points under Datum Point feature, reference one of them by another feature (or components placement), and later pattern it by the while array.

This just adds 3D aspect to point pattern.