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hole call out help

fdefilippi
1-Newbie

hole call out help

Greetings:

I'm really struggling to understand Creo's drawing module and one of the issues is hole callout.   I was told that the drawing mod.  does have that ability and you have to use 'Show Model Annotation"  weird but okay.  So I found out a how have hole call out show but the callout is not what I was expecting.   Need some help on this been at it for 1/2 cay and still can figure it out.


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1 ACCEPTED SOLUTION

Accepted Solutions

To close this community thread on Hole Callout Format

 

Summary of the exchanges and proposed solution, also summarized in article CS28399:

  • Default callout for Standard holes can be customized in the CALLOUT_FORMAT section of associated .hol file, located in the <Creo Installation>\Common Files\text\hole folder:
    • For example C:\Program Files\PTC\Creo 8.0.0.0\Common Files\text\hole
    • The configuration option hole_parameter_file_path can be used to set the location of custom .hol files
  • Under the CALLOUT_FORMAT section you can use different tokens that represent parameters or symbols, for example &DIAMETER that represents the Drill Diameter or <ctrl-a>v<ctrl-b> for the counterbore symbol
    • A list of tokens can be reviewed in the Creo Help Center, like here for Creo 8.0 (note that some parameters may not be applicable for previous releases).
  • This section will apply to all Hole types, so unwanted information displayed for some configurations:
    • If some tokens are not required when the Hole state changes (eg adding a Countersink or setting the Thread depth Through all) you can create a table in a new DEFAULT_CALLOUT_FORMAT_DATA section at the bottom of the hole chart file.
    • The different callouts can be defined for each combination.
    • Refer again to Creo Help center here for more details
  • Specific examples are discussed in the different replies oh this thread

View solution in original post

28 REPLIES 28

PTC Creo Parametric uses a lot of lookup tables to come up with parameter names.  Some of these are managed internally which makes following a particular parameter (variable) hard to follow or use at will.

One of the lookup table sets are the hole tables.  They have the text version of the text that will show up in the dialog box for hole annotation.

Sometimes it is worth the time investment to make the tables do what you want.  For me, this isn't the case as I have many clients all wanting their own.  I simply create notes with the annotation I require for each client.  It is still associative if I build the note using available parameters.

Word of caution if you go changing Creo system level files... these are easily lost in a software update.  Either point your config.pro to a location outside the Creo folder structure or save the library to a backup location and remember to replace them when the updates occur.

Is it this table?

Hi,

Hole definition files are text files with .hol extension in hole subdirectory.

In my installation it is C:\PTC\Creo2_M070\Creo 2.0\Common Files\M070\text\hole​ directory

MH


Martin Hanák

Martin-

I located the file, but I don't know what to do next.  Can you or someone walk me through this?

Thxs

‌The parameters used for the hole note are the columns found in hole tables. The hole note itself may include more parameters than what you want as the note is formated so that it displays the relavent parameters depending on whether you are defining an English or metric standard thread. Try looking up hole table parameters in the help, it lists the parameters for each thread type. The note itself is defined in the hole tables. For symbols, such as the depth symbol, you need to determine the ASCII code to be used.

I usually don't remember what's relavent either so I use control "x" to cut after maybe &STD_HOLE. Then check the drawing and go back and add part of what you cut if missing something and/or if good then just add the depth symbol with the "d" number for the depth dimension in the part. It gets me there, wish ptc made that easier in creo Also the next holes are easier once you get the hang of it.

Attached is part of the default UNC table and the reference to the help documentation as to what parameters are used:

UNC Hole Table.JPG

Callout Format.JPG

You specify the parameters you want below the CALLOUT_FORMAT.

Thank you.

I believe I'm pretty much in over my head on this. 

It's very much like creating notes with displayed dimensions. I'd say first determine whether you are going edit the standard tables or create your own. If you create your own, make sure THREAD_SERIES in the header is set to what you want to appear in the thread specification drop-down of the hole feature, as this is what is shown, usually the same as the hole table file name.

Under CALLOUT_FORMAT add the parameters and other text and symbols you want to show, any column heading in the hole table file is valid. Try starting with 1 or 2 parameters such as:

&FASTENER_ID &THREAD

then try adding symbols:

<CTRL-a>x<CTRL-b> adds the depth symbol. Try different values to see what you get, I haven't found a list that shows what letter gives which symbol.

Also look up Formatting Thread Notes and there is a link to the valid parameters for use in the CALLOUT_FORMAT.

Hi Kevin-

Okay some updates.  4 hours later and I figured out how to add c'bore based on the screen shot below.  So my next question is if I wanted to add c-sink how would I do that?  would it be the next line below?

You could keep the call out all on one line if you wanted the forward slash lets the system know you want something on a new line. Try:

<CTRL-a>w<CTRL-b><CTRL-a>n<CTRL-b>&CSINKDIAM X &CSINKANGLE

Not sure if its working do I add the text you recommend like this on the screen shot?

<CTRL-a>w<CTRL-b><CTRL-a>n<CTRL-b>&CSINKDIAM X &CSINKANGLE

Because I get this in the model when adding the line you mentioned.   

All you need to add is a forward slash, /, at the end of your original text and the text you added:

&CBORE_DEPTH[.2]/<CTRL-a>w<CTRL-b><CTRL-a>n<CTRL-b>&CSINKDIAM X &CSINKANGLE

Kevin-

Still not working  please see the screen shot below

I add the text line you mentioned

In the 3d model I get this then

Then in the drawing call out I get this.

As you can see its not correct.. suggestions?

Since you have a hole table file with mixed hole states add the following to the bottom of the file:

DEFAULT_CALLOUT_FORMAT_DATA

HOLE_TYPE  THREAD  DRILLED_DEPTH  THREAD_DEPTH  CSINK  CBORE  EXIT_CSINK  CALLOUT_FORMAT

TAPPED  YES  VAR  VAR  NO  NO  NO  &FASTENER_ID

TAPPED  YES  VAR  VAR  YES NO  NO  &FASTENER_ID/<CTRL-a>w<CTRL-b><CTRL-a>n<CTRL-b>&CSINKDIAM X &CSINKANGLE

TAPPED  YES  VAR  VAR  NO  YES  NO  &FASTENER_ID/<CTRL-a>v<CTRL-b><CTRL-a>n<CTRL-b>&CBOREDIAM <CTRL-a>x<CTRL-b>&CBOREDEPTH


This should format the note based on the hole features you have.


You can remove the information from the CALLOUT_FORMAT line at the top.

here?

  didn't work

My guess is you need to try a different value for the DRILLED_DEPTH and THREAD_DEPTH. Start by changing the DRILLED_DEPTH value to THRU_ALL. These values come from how you define the hole. If these values don't match the system defaults to using the default call out.

Here is a pic of three holes with the DRILLED_DEPTH set to THRU_ALL and THREAD_DEPTH set to VAR.Thread Notes.JPG

After redefining the holes in the model to be variable the default note is used.

Thread Notes-2.JPG

Another thing that may be causing what you are seeing is when you redefine the hole or change the note format in the *.hol file is that the notes may not automatically update, make sure to sellect reset on the Note tab and see if that updates the note.

After changing the DRILLED_DEPTH value in *.hol file to VAR for all three hole definitions, edit definition of hole 3 and reset note.

Thread Notes-3.JPG

I still can't figure this out and its becoming very frustrating.. what other methods are there for creating a note hole on a drawing?

StephenW
23-Emerald I
(To:fdefilippi)

I never use the hole note. I show my dimensions and then edit the diameter dimension to show all the dimensions as I want them too.

If you are still interested in trying maybe this will help:

CALLOUT_FORMAT is good for a generic note for holes that always have the same features and their notes will be the same. Because you are wanting to use different features with the holes you need to use the DEFAULT_CALLOUT_FORMAT_DATA to specify the holes configuration and the parameters you want to see for use with that configuration. I'm attaching images to show where the DEFAULT_CALLOUT_FORMAT_DATA is getting information from:

Hole-1.png

If you had the following in your *.hol file:

DEFAULT_CALLOUT_FORMAT_DATA

HOLE_TYPE  THREAD  DRILLED_DEPTH  THREAD_DEPTH  CSINK  CBORE  EXIT_CSINK  CALLOUT_FORMAT

TAPPED  YES  VAR  VAR  NO  NO  NO  &FASTENER_ID &THREAD_SERIES-&THREAD_CLASS

you should get 1/4-28 UNF-2B from the image above.

For this hole definition and the DEFAULT_CALLOUT_FORMAT_DATA above:

Hole-2.png

you should get the Creo default note. The reason being is you have deselected the thread and it is now a DRILLED hole with no thread.

If you want to change the hole to the following:

Hole-3.png

and you want to keep the note format from above you need to add another line for another hole configuration otherwise you would get the Creo default note. In the image above two things were done, the DRILLED_DEPTH was changed to THRU_ALL and a countersink was added. The new line is added and modified as shown:

DEFAULT_CALLOUT_FORMAT_DATA

HOLE_TYPE  THREAD  DRILLED_DEPTH  THREAD_DEPTH  CSINK  CBORE  EXIT_CSINK  CALLOUT_FORMAT

TAPPED  YES  VAR  VAR  NO  NO  NO  &FASTENER_ID &THREAD_SERIES-&THREAD_CLASS

TAPPED  YES  THRU_ALL  VAR  YES  NO  NO  &FASTENER_ID &THREAD_SERIES-&THREAD_CLASS/<CTRL-a>w<CTRL-b><CTRL-a>n<CTRL-b>&CSINKDIAM X &CSINKANGLE


Any holes that don't conform to the two configurations shown display the Creo default note. If you want to use *.hol files and format the notes to what you want, you need a line for each hole configuration.


In the following I get the default Creo note because the hole is THRU_ALL not VAR, so the hole definition doesn't match the format data above:


hole-4.JPG


To get the correct note for a thru hole the following line needs to be added to the DEFAULT_CALLOUT_FORMAT_DATA:

TAPPED  YES  THRU_ALL  VAR  NO  NO  NO  &FASTENER_ID &THREAD_SERIES-&THREAD_CLASS


If you wanted a blind hole, you would change the DRIILED_DEPTH selection and you may or may not need to select Reset on the Note tab since it may or may not update automatically. You don't need to add a line to the *.hol file because it's already there.


If it's still not working I'd need to know the hole configuration to help with the note format or know where exactly the confusion lies. The only other thing I can say is start with one line in the DEFAULT_CALLOUT_FORMAT_DATA, change the parameters and modify the hole in various ways to see what it gives you.

Thanks Kevin-

I'll look into this tomorrow.  In general this is far more complex than it should be compared to all other CAD systems I've ever used.  A simple hole tapped or not with a depth shouldn't require all of this..  Thanks for your time and effort and I'll look into this

Thanks

Unfortunately, everything in Creo is like this from Welding to Cabling and Piping.

Yes I'm seeing this as a 4 month user of this s/w. most things taken for granted in past CAD packages are not intuitive as this one.. wonder why?

Perhaps the question I should ask is does anyone have an ISO.hole file they can send me so I can figure out how to do this?  

thanks

Frank

Try this and see if it works. Start out with a variable depth hole adding the countersink and counterbore individually to the hole. The hole note should display the thread call out as the default and when you add a countersink or counterbore it should add the appropriate information. After you see that work change the hole type in the hole feature to THRU_ALL, when you do that the only thing that should display is the thread call out. If you add the countersink or counterbore you should only see the thread call out displayed, save your file and close. Go to the *.hol file and edit the DRILLED_DEPTH value for the desired hole to THRU_ALL, save *.hol file and re-open Creo. Edit the definition of the hole, select the Note tab, and select Reset. If the sequence was done right you should see the correct information displayed.

I'll look into this.  I think I've cost my employer too much trying to figure something simple as this out.

To close this community thread on Hole Callout Format

 

Summary of the exchanges and proposed solution, also summarized in article CS28399:

  • Default callout for Standard holes can be customized in the CALLOUT_FORMAT section of associated .hol file, located in the <Creo Installation>\Common Files\text\hole folder:
    • For example C:\Program Files\PTC\Creo 8.0.0.0\Common Files\text\hole
    • The configuration option hole_parameter_file_path can be used to set the location of custom .hol files
  • Under the CALLOUT_FORMAT section you can use different tokens that represent parameters or symbols, for example &DIAMETER that represents the Drill Diameter or <ctrl-a>v<ctrl-b> for the counterbore symbol
    • A list of tokens can be reviewed in the Creo Help Center, like here for Creo 8.0 (note that some parameters may not be applicable for previous releases).
  • This section will apply to all Hole types, so unwanted information displayed for some configurations:
    • If some tokens are not required when the Hole state changes (eg adding a Countersink or setting the Thread depth Through all) you can create a table in a new DEFAULT_CALLOUT_FORMAT_DATA section at the bottom of the hole chart file.
    • The different callouts can be defined for each combination.
    • Refer again to Creo Help center here for more details
  • Specific examples are discussed in the different replies oh this thread
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