Point locations

[dveljkovic]

Hi guys,

I have several points attached to different surfaces on assembly model. I want to make a table (in drawing) with XYZ coordinate measured from XYZ CSYS for each point. How can I do this?

Thanks.

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[TomD.inPDX]

What if you insert an empty part in your assembly with the default CSYS where you need it. Now activate the part in the assembly and create datum points on top of the already defined points in the assembly.

Now open the part and export it as IGES. The iges file can be read and the points will have the XYZ coordinates in the file. Now load the IGES data into an excel file (formatted) and read that back into a table (we can do that, right?).

[dveljkovic]

Antonius, it sounds interesting but the only problem is that it will not update itself once points change locations. And that can cause a lots of problems.

[TomD.inPDX]

Ohhhhh... well that's another story. True, the IGES method is suggested by PTC in creating datum curves through points.

I think to manage a parametric relationship you will have to think outside the box. I'm going to get very wild in this thought and would be happy to see others come up with a better plan.

My idea is to do exactly as before, make a part with "duplicate" points. This is not required but maybe easier to manage.

In the new part, create sketches that -somehow- provide reference dimensions to the datum points from the csys. These dimensions, through several sketches (one for each of the 3 planes) will now have the data for each point. You can either build the data into relations or use the dimensions directly in a table. In a drawing, I would even suggest assembling just the point-part and activating it to obtain the table data.

I am not doing this so I am just thinking outside the box. Let me know if any of this sounds appealing.

And if someone has a better idea... PLEASE ENLIGHTEN US

[ptc-5008082]

Whether this solution is helpful will rather depend on whether I have fully understood your query......

If the points whose co-ordinates you want to show are at the assembly level – i.e. APNT0, APNT1 etc. then you can create a hole table in the drawing of the assembly.

You will need to have a co-ordinate system in the drawing view that has an X axis pointing to the right and a Y axis pointing upwards and the Z perpendicular to the screen.

Then you can use Tools > Hole Table in Wildfire or Table > Hole Table in Creo select the co-ordinate system and it will populate the table with the x, y and z co-ordinates with respect to the csys you chose.

If the points are in the parts then you will need to somehow move the points to the assembly level, as Antonius suggested by putting assembly level points on top of already created points.

In Wildfire this solution is semi-parametric as the table does not update automatically, you have to create the table again – but it is few clicks.

If you are in Creo then the table will update on a Regenerate in the drawing (rather than an update drawing view)

The interface in Creo is much improved and you can save table configurations and all sorts.

[dveljkovic]

I will try this method. Was thinking about it but woking with Creo's hole table is very awkward for me. I guess, missing a clear instruction from Creo on what has to be done to achieve what you need is the biggest flaw Creo has.

[TomD.inPDX]

I was really hoping there would be a way to get the data from already existing points. Sounds like there is.

Charlotte, how does the table know to look for the points to populate the table?

[ptc-5008082]

It’s the magic point pixies Antonius

No, really, it is based on the type of feature, back in version Pro/E 14/15 this table literally only worked on holes created with the Hole functionality, over the years they have added on axes and points.

You don’t have much in the way of control, you create the csys so that the orientation is correct for the drawing and once it has that csys it indiscriminately looks for features of the chosen type.

It will then display the information that it can about the type, i.e. holes get x, y and diameter, points get x, y and z and I think from memory axes get x and y.

You can create notes on the drawing to automagically label the holes too so I used it a lot for side member drilling drawings in days gone by.

[TomD.inPDX]

Very good to know, Charlotte. Thanks for the detailed information!

[BrianMartin]

I would agree that the hole table feature is probably the best way to go... but there is another way.

You can always simply perform a measurement and save it as a feature. You have options to automatically generate and keep parameters for the X, Y, and Z coordinates. You can then access these parameters in your drawing table.The downside of this technique is that you can only measure from the csys to one of your points per feature. The upside is that you do not need a physical datum point for this to work. You can simply select vertices and forego the points if you wish.

In Creo the new Measurement Summary tool does allow you to make multiple measurements from the CSYS to numerous points/vertices simultaneously... but you cannot save them as a feature. That sort of kills this as an option.

But to get super intricate on this issue and drop some archaic little-known information... there is a way to make numerous measurements in one single feature and access them later in a table, relations, or parameters. Even though the feature has been removed from the ribbon, you can still access the Evaluate Datum feature. With an Evaluate feature, an old type of measurement that could be saved and recalled later, you can access data from numerous measurements simultaneously. You can even mix and match angle measurements, distances, curve lengths, areas, etc. This is not possible even with the new measurement tool.

The upside is that all of your measurements can be located in one feature. You could easily create a table that will reference the measurement parameters... and all of this will work in Wildfire or Creo. The downsides are that you need to name each measurement set, you must create a new measurement between each CSYS and it's accompanying point/vertex, and while I could get distance, I couldn't get X,Y, and Z data using this method.

Anyway... as I said the hole table is probably the best... but I like the method of pulling data from measurement parameters. It may not be the most useful in this case, but it's a very little used technique that is never taught. I'm all about learning and using the very fringe bits of Creo in situations where it's warranted. I thought this might be a good place to at least bring up the topic of Evaluate features in case it can be helpful to someone else. To use it in Creo you must set allow_anatomic_features to yes in your config.pro. You also have to type "Evaluate" into the Command search to find it.

Thanks!

-Brian

[ptc-5008082]

Brian, how do I "easily create a table that will reference the measurement parameters"??

Evaluate features I have and I can extract the values into relations through FID but how to I tabulate all this good stuff??

I am also a fan of “learning and using the very fringe bits of Creo”

[dveljkovic]

This is where I get pissed at Creo. Why the hell I have to use Feature ID when I should be able to use name of the measurement for relating to the value in the measurement. For ex., something like this: X_COORD:PT_01 instead of this X_COORD:FID_1798. Which one is easier to remember?

[ptc-5008082]

the FID is the feature ID but that can be the name of the measurement feature, so for example I have measurement named 'length' inside feature called 'eval' then I can put

length:fid_eval

[dveljkovic]

Yes. You can do just like you said. So, here is an example of mine. I have a datum point Z1. I can get XYZ coordinate from assembly CSYS and save the measurement as Z1 as feature (not analysis). Now, if I want to access X_COORD of this measurement I type &X_COORD:FID_Z1. Everything is fine. BUT, as soon as I close the note properties, everything turns into &X_COORD:FID_1798:1?!? Why creo change it?

[Dale_Rosema]

... and have to learn the finge bits of Creo......