V4 ordinate Dimensioning 1

[rickyt]

Is it possible to dimension in Catia v4 with the ordinate style of dimensions. Can it be set up thru drwstd.

Thanks for any advice on how to do so!

 

[jackk]

Ricky,

There used to be a COORD menu in the DIMENS FK. but I think they took it out and replaced it with a command /COORD (or maybe /m COORD). (sorry, but I don't have access to V4 anymore, so I'm going by memory) I think one of the European auto companies has written their own command, /KOORD, to dimension to their own standand.

Hope this helps. If this isn't the kind of dimension you want, could you attach an image of what you're looking for? I think you might be able to use DATUM dimens for a another type of ordinate dimensions.

.....Jack

 

[rickyt]

Jack, Thanks for your Response.

I will try what you have mentioned.

I need to dimension alot of holes on a tooling plate.
Ones I have done in the past have been so clutered and its hard for the shop to read. I would like to have the numeric value right next to the feature.
what I am looking for is to be able to pick my zero corner then pick a hole, the result would be one horizontal dimension and one vertical dimension from the zero corner.
There would be no dimension lines or arrowheads, just a small extention line for each dim. coming from the hole center with the value along side it. The dimension text
would be horizontal for the up/down dimesions and vertical for the left/right dimesions.
I have gone thru some of the iua macros today and found one that will probably work. It was coord*****? (there where only 3 of them that started with coord).
It is probably the one you where thinking of.

What it does is in draw mode asks for what axis to take dims from then asks what points to dimension. It puts a X ##.## and a Y ##.## The number of decimal places etc is dependent on your dimension parameters, it also puts an arrowhead symbol pointing to the point, which can be eliminated by setting up the dimension parameter symbol as "no symbol" This is pretty much what I was looking for other than I would like to get rid of the X and Y prefix on each dimension, but it will do.

 

[jackk]

Ricky.....

Yes - you found the macro I was trying to describe. I'm glad to hear it's what you were looking for.

If you have some free time, you might want to try to modify the COORD macro to get it to do exactly what you want. Copy the old one first, so you don't destroy it. Then, use MACRO+EDIT to see the code and change it. MACRO+EXECUTE will let you test it, and it will stop when it comes to an error. I'm not a programmer, but I was able to customize other macros this way, and it was pretty easy.

From your description of the part, I'm curious if you've tried to dimension all the holes with a hole chart? I've done this in the past with parts with many holes and it does make it much easier for the shop - but it's alot of work for the drafter. The trick is to group and label all the same size holes ('A' might be .250 DIA, 'B' might be .125 DIA, 1.00 DEEP, etc.) If you have many parts like this, you could use attributes to label the holes and write a REPORTER to automatically build the chart. (before you do this, make sure REPORTER has the ability to include the X and Y coordinate - sorry it's been awhile since I did this with V4)

.....Jack

 

[Catusr]

rickyt,

If you are creating a point chart for the locations of hole, I,ve devoloped a way to create a point chart of x,y,z or just x,y locations if preferred, in seconds. It take a 15min. of preperation time, but it will create a chart of any number of points in seconds.
It has saved my hours and hours of typing, and my company money. The best thing about it you can't get the point chart wrong.
Let me know if this is what you want.

Catusr

 

[belvedere64]

Catusr

I am in the tubing buisiness and what you are describing is exactly what I need. We define the planar bends with intersection points and radii. I did not buy the tubing module, but I am having fun with PARAM3D. Typing is the worst thing that I do. The check process is murder! Any help is greatly appreciated.

Thanks

Mit Freundlichen Grüßen,
Thank You,

K. C. Takacs
der Entwicklungsingenieur/Design Engineer

 

[rickyt]

http://engr.bd.psu.edu/ncs/Linear_to_Ordinate.html

Is a example of what I have been looking for in regards to ordinate dimensioning, the bottom picture shows a ordinate dimension of 1.50, this is what I would like to do in catia v4. This would eliminate much clutter without having all the extra extension and dimension lines. So if I was to do a layout, I would have zero/zero identified, then a seperate x and y dimension along side each hole. these dimensions would just have the small extension line from the center and the dimension value, nothing else.

 

[rickyt]

the above message should have not mentioned the bottom picture, its the second picture down from the top.
see some of the other pictures for examples of ordinate dimensioning, I just want to do it in a true view, not a isometric, like they have shown in some of the pictures.

 

[BrianShipston]

Ordinate Dimensioning is available in CATIA V4 under the DIMENS2 function.
If you have a standard CATIA installation there is an icon that looks something like this O-->|-->| This is used for making ordinate (Cumulate in CATIA) dimension systems. The Cumulate section of the parameters enables you to modify the text location, text orientation etc.

If you have any further questions feel free to contact me.

brian@tbmtech.com