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Hatching Creo 4

Level 8

Hatching Creo 4

Apologies if this is documented elsewhere, but I haven't yet found it

 

 I have  two years worth of students learning Creo 4 (M020) at present  and we seemd to have hit a problem with drawing and cross-sections/hatching. I am not sure I fully understand, but it seems that in some cases you need to use 'scale' to change the spacing and in others the traditional 'spacing' option. I think it is related to section you use for the x-section, is that right? If you are using a start-part/component with a section defined on a previous version of Creo (Pro/E)  you need to use spacing. If it is a new section, even on a old component you need to use scale.

    This can mean depending which datum plane you chose on ONE model the hatching behaves in a different way. Is this correct?

 

  If yes, it would explain the confusion this is producing with the students. Please say there is a config.pro option, that I haven't found, that automatically redefines one of the types of sections (I assume old) to behave like the other.

 

 This is relatively urgent I have another 90 students attempting this class on Thursday!

 

  Many Thanks

 

7 REPLIES 7

Re: Hatching Creo 4

There are two kinds of crosshatching.

 

The old one which only uses parallel lines and can apply line styles to customize the appearance. It only has spacing and angle to control the way it draws.

 

The new one which uses 2D graphics of any vector kind that has been converted to a .pat format to fill an area. Since it is 2D, spacing makes no sense as there isn't any way to tell which spacing.

 

The technology between the two is entirely different so they cannot behave like each other. It has nothing to do with which datum plane is chosen.

 

"You can set the default crosshatch pattern file type as pat or xch using the configuration option default_hatch_type." Read the following (The server is screwed up. I had to reload about 10 times to finally get the page to come up. If it takes more than 2 seconds, hit the reload button again.)

 

http://help.ptc.com/creo_hc/creo30_pma_hc/usascii/index.html#page/fundamentals/fundamentals/fund_fou...

Re: Hatching Creo 4

Thank you for the fast reply, currently I am away from my creo seat to try the config and also a higher speed link to try and read thedocument . Apologies about using the term datum, it should really be section, but of course often based on a  d datum. The confusion being seen means that two identically looking views on the same drawing can behave differently depending if the section being used is new or old. As all our parts/assemblies generated for the last 15+ years have at least predefined sections on x,yz=0 it would be a lot of work to redefine them to fully move over to .pat/scale hatching. Thankfully our mapkeys work identically with both types, it is the confusion seen by new users when one view/section uses spacing and the next may be scale just depending if the section (possibly based on the same [datum] plane) is being used. I haven't yet confirmdd, but I think we had some situations with two types seen in local sections on the sameview

 

Re: Hatching Creo 4

Apologies about the typos in the previous reply, working on a very slow broadband line.

 

However, confirmation you can have two local sections on one view with different types of hatching, with spacing accessed either via Spacing or Scale.  While I see the reason it is very confusing to new users.. especially as it involves using the excellent Pro/E menu structure 8-). [Our students still understand the text based meus quicker than those with 'thousands' of tiny/similar icons..!] The only problem is that it isn't so easy to re-configure the menu to have a single Icon or Word to cover both scale and spacing.

 

  Can I assume that the Spacing route will slowly be deprecated by PTC so it would be good to move to the Scale as soon as possible?

 

  Many Thanks for your help

 

Re: Hatching Creo 4


@cadcam wrote:

Apologies about the typos in the previous reply, working on a very slow broadband line. 


I never knew that typos were related to a slow broadband line ;-)

 

Seriously, I would look into defining the Cross Hatching in to the Material Properties.

 

Related

https://support.ptc.com/help/creo/creo_pma/usascii/index.html#page/model-based_definition/To_Define_...

 

http://help.ptc.com/creo_hc/creo30_pma_hc/usascii/index.html#page/detail/Determining_Crosshatching_P...

Re: Hatching Creo 4

With further testng I now believe this may be an issue with 4.0 M020. default_hatch_type is not accepted as an option within config.pro and the ability to switch between xch and pat in the Hatch menu manager is missing. However, it seems to be available in M040. Unfortunately we are unable to upgrade at present 8-(

 

 

Re: Hatching Creo 4

Hi,

 

another Creo 4.0 problem related to cross-hatching is the fact that Common Files\text\crosshatch directory contains .pat files, only ... .xch files are not available in Creo 4.0 installation.


Martin Hanák
Highlighted

Re: Hatching Creo 4

I know this thread is related to sections, but I'm having a similar problem with cross-hatched sketches in part modeling. In old versions of Creo I could chose "spacing", and that allowed me to have the same line spacing for different sketched areas on the same part or in different parts of an assembly.

 

I'm on 5.0.0.0 right now and "spacing" is not available, only "scale" but this means that to have a consistent x-hatch spacing for parts that have different sizes I have to guess and keep tweaking that **bleep** parameter. I have a case open and besides asking the PM for more info and a link to a very old SPR I didn't get much. I really don't get who would benefit from such a silly way to define x-hatch in part modeling....