# square peg in a round hole

#### bhayden

##### New member
I have a thin metal cage that gets assembled to a circuit board. The pins are rectangular in cross section and of course the holes in the PCB are round. I figure adding an axis throught the center of the leg that will be inserted into the hole is the best practice for assembly. My question is, is there a slick way to find the center of the material thickness or should I just measure, offset two planes half the width and material thickness and create and axis at the intersection of the two planes? Seems like the a long way around.

View attachment 22

Bernie Hayden

G

#### Guest

##### Guest
In sketcher, add an Axis Point (Sketch > Axis Point) at the center of the square section. This will create a datum axis through the center of your square protrustion that you can use for an assembly reference.

#### bhayden

##### New member
Oops, forgot to add one critical piece of information. This part is imported geometry from a vendor supplied model. So I'm very limited in what can be selected. I guess what I'm after is something like create a plane half way between two surfaces or perpendicular to the mid-point of an edge. Using #Analysis #Measure and make datums isn't too bad if the results even thousands or an inch (or hundreds of a millimeter) but it would be nice to find the mid-plane using geometric constrains rather than hard numbers and make datums.

-Bernie-

##### Moderator
Create an axis, then create 2 datum-planes-on-the-fly to define the axis.

To eliminate any measuring or relations, define the first plane through two diagonally opposite edges on the leg. Then define the other plane using the other pair of diagonally opposite edges... Axis should end up right in the middle of the material.

-Brian

#### miked

##### New member
could you pick an edge of one side that defines the thickness and use it to create a datum point using length ratio (use .5) then create a datum plane thru this parallel to the outside face of the part (or another datum).

This way if the part ever changes thickness the plane always stays in the center.

Mike

#### bhayden

##### New member
Brian,

Your solution of creating an axis defined by make datum using two planes through edges works great. No extraineous features left clutering up the model and it's parametricly related to the model. Chalk up another one for Make Datum

Mike,

I'm not familiar with the method you suggested. I tried several methods of creating a datum point. Offset Point seems to be closest to what you describe but I don't know how to enter a length ratio. Please explain.

-Bernie-

#### dougr

##### New member
Axis thru two planes is how I would do it with make-datums.

Why did PTC get rid of DOTF in misfire, seems that no one left there has much in the way of intellect..

#### miked

##### New member
It depends which version you are using.

In 2001 I think it goes something like

Insert, Datum, Point, On Curve, Length Ratio

I could be wrong though Ive been using wildfire for awhile and I used mapkeys in 2001 so I may not have the picks right.

Length ratio is exactly as it sounds, .5 will put the point at the middle of the curve. The only problem is when you want something other than .5 you cant always predict which end of the curve is the beginning.

Mike

##### Moderator
Regarding my earlier post:

Create an axis, then create 2 datum-planes-on-the-fly to define the axis.

This works in Wildfire as well as 2001. The difference is that the two datums-on-the-fly will show up in the model tree instead of being 'hidden' as they used to be with the make-datum' type of datum-on-the-fly.

-Brian

#### dougr

##### New member
Yeah with two extra features.

Not nearly as clean.

Now imagine if you had to pattern this axis - you have 3 features per pattern instance, not one and you have to screw with groups now.

Does misfire automatically group features created in this manner ?? ie Are the planes grouped with the axis ??

FYI If you see them in the model tree then they're not on the fly.

##### Moderator
Regarding groups:

Yes, Wildfire automatically creates a group containing two datum planes and a single axis. The datum planes are 'hidden' by default so they don't clutter the screen.

Regarding patterning:

for this example, if we assume that the 'peg' is a patterned feature, then I would simply select the axis group, right click and choose 'pattern' and then 'reference'. Then the axis is automatically patterned based on the pattern of its parent. looks good to me.

Regarding on the fly:

I've never seen an official definition, but in my experience, the term on-the-fly refers to any supporting feature you are able to create while in the middle of creating another feature. So in my experience, both Make-Datums and Asynchronous-Datums (as PTC calls them) are on-the-fly features ... not just Make-Datums.

The one complaint I have with the new functionality is that the patterning functionality of groups is limited only to general. So patterning features containing on-the-fly datums in Wildfire works, but you can't use identical or variable. This is obviously a performance hit on complex patterns.

-Brian

##### Moderator
By official, I meant PTC. We, as users, can call them whatever we want...

But, no matter what you call them, you are still able to create datum features while in the midst of creating another feature. You can call these on-the-fly or as-you-go or on-the-run... it makes no difference.

I can't understand why people obsess over the semantics.

I've even seen people complain about the missing make-datum menu pick who didn't even realize what the implications are. They were just so used to picked that menu-pick that they got all bent out of shape when they heard it wasn't there anymore. I suppose they're also upset that sketches now show up in the model tree under the part feature.... Some people just don't handle change well I guess.

Bottom line from what I've seen so far:

Con: Resulting group gets a stupid automatic name (AUTO_GROUP)

Con: General patterns only (for groups in general)

Pro & Con: Datums are no longer embedded within feature, but instead show up as reusable features on model tree. For me, personally, this will be more of a Pro than a Con.

-Brian

#### bhayden

##### New member
I haven't played with WtF enough yet to have a strong opinion on the DOTF issue. Although I'm a big believer in if it ain't broke don't fix it!. The creation of groups seems like a problem mostly because you can't group groups (unless they fixed that) and group creation is often required because of ProE's lame patterning methodology.

Showing in the model tree doesn't sound all bad and from what I understand they're hidden by default. My question is do the datums show up on the model. If so then that's a major CON in my book since one of the most appealing features of make datum is it cuts down on clutter in the model display. I suppose there's a crafty work-around for this with layers but; if it ain't broke, don't fix it.

Bernie Hayden

XKL LLC

(boy has this thread gone off topic

#### dougr

##### New member

Boy, you're easily annoyed - chill out..

It's not a matter of semantics when removal of DOTF triples and quadruples the number of features in a feature pattern.

It's not semantics when we have to bugger about with groups now.

It's not semantics when our patterning options have been removed.

It's not necessarily semantics when people are being accurate & precise - some members on this site would greatly benefit by being more accurate and precise in both their questions and responses.

I handle change as well as the next guy and probably better than you - changes aren't always forward and this one is definitely a step in the wrong direction.

Have you ever used DOTF and if so what for ???

##### Moderator
Doug,

ouch... I'm not at all annoyed, and I hope you didn't think I was referring you you specifically when I said that some people are resistant to change. I am referring to the background chatter of users who've never once started up WF, but who still complain incessantly about issues that they don't fully understand... at least that's what I was trying to convey...I certainly didn't intend to challenge your manhood or anything...

I agree with you on the whole groups thing (I think I expressed that in my previous post), If PTC could retain the ability to create variable and identical patterns afterwards, I don't think I would have been such a big deal.

As for accuracy and precision, maybe we should start using PTC's official term Asynchronous Datums Planes for the only type that exists now in Wildfire (along with asynchronous axes, points. etc.).

For others reading this thread, here is PTC's explanation of this topic that has gone horribly off track:

http://www.ptc.com/cs/tpi/117375.htm

-Brian

##### Moderator
Bernie,

In response to your question, no, the not-on-the-fly datums don't show up in the model. They appear in the model tree (inside a group), but they are hidden and the icons are greyed out. I believe that you can unhide them, but I didn't think to try that...

They actually appear briefly in the graphics window when you finish the feature, but then they disappear.

I am also assuming that they STAY hidden the next time you open the model, but of course, I forgot to try that as well. Normally, hiding features in 2001 & WF is only temporary and hidden features revert back to unhidden the next time you bring them into session.

-Brian