How to do a section in an axonometry wiew in drawing?

[lnessi]

Hi

I have to do an axonometry wiew but with a section! And if is possible in shading with edge rappresentation as in the picture below!

I did this saving the jpeg file and putting it as object in drawing, is the only way to do it?

Thanks!

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[MartinHanak · Accepted solution]

Luca,

you can use following procedure:

1.] add x-hatching default real number parameters into your model (Tools > Parameters)

default_xhatch_angle

default_xhatch_spacing

See details in http://help.ptc.com/creo_hc/creo30_pma_hc/usascii/index.html#page/pma/fundamentals/fund_four_sub/To_Set_the_Default_Spac…

These parameters drive x-hatching properties displayed on the drawing.

2.] create Zone (3D x-section) in your mode ... see myzone in my model (created in CR2 M070)

3.] in drawing view properties in Sections category set 3D cross-section myzone

You cannot modify x-hatching of 3D x-section in Drawing mode!!!

MH

[lnessi]

It works thanks!!

I have a little question more!

I have to do it in an assembly, is possible to exclude any components? an example screws, nuts exc...

Thanks!

[MartinHanak]

Luca,

I tested below described procedure using assembly with 2 components.

In Assembly mode:

1.] I defined zone

2.] I defined layer and put unwanted component into it

3.] I hid the layer and saved layer status into layer state (Layer_State002_1Comp)

4.] I defined combined state (Comb0001 referencing Layer_State002_1Comp)

In Drawing mode:

5.] I created view referencing combined state (Comb0001)

If you do not understand my procedure, please let me know. Tomorrow I can prepare example data for you.

MH

[lnessi]

I understand the procedure, but maybe i made a mistake on the question formulation!!

The meaning was that i want to exclude some parts from the section hatch and continue to see these un-cutted!!

Some parts have to be sectioned an some no.

It's possible do this?

Sorry for the mistake; Thanks!!

[MartinHanak]

Luca,

in Drawing mode doubleclick xhatch area.

Following menu opens.

Use Pick, Next, Previous command to select requested component.

Use Exclude command to remove sectioning from selected component.

Use Restore command to restore sectioning of selected component

MH

[MartinHanak]

In Assembly mode you can edit definition of x-section to remove sectioning from selected component.

If you create a drawing view using such x-section, Creo maintains component status defined in Assembly mode.

MH

[lnessi]

Thanks!

My final objective is to do this!

An axonometry wiew with section and with some part not sectioned, in shading with edge rappresentation in drawing as in the picture.

Is possible?

Thanks

[MartinHanak]

Yes it is possible.

MH