drafting/detailing 2

[pamccrac]

is there a way to insert weld symbols on a drawing?

 

[Heckler]

View > Show & Erase

Heckler
Sr. Mechanical Engineer
SWx 2007 SP 3.0 & Pro/E 2001
XP Pro SP2.0 P4 3.6 GHz, 1GB RAM
NVIDIA Quadro FX 1400
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(In reference to David Beckham) "He can't kick with his left foot, he can't tackle, he can't head the ball and he doesn't score many goals. Apart from that, he's all right." -- George Best

 

[robertib]

The way Heckler says assumes that you have the weld symbol in the model. If not, the way to get them is:-

Insert > Drawing Symbol > Custom

in the drop-down box, go to System Syms - the weld details are in the folder weldsymlib.

 

[pamccrac]

thanks Robertib, i will give that a try!

 

[pamccrac]

i have other problems now...
I have started a drawing and found that the part is in metric but I want imperial. so I went to the part setup and changed the part to imperial and verified that my primary drafting units is imperial, but I still get metric dimensions. Although if I use the Distance tool I get imperial. Do I need to start over?

 

[mjcole]

When you change the parts units you are given two options.

Same Dimensions 25.4mm becomes 25.4in
or
Same Size 25.4mm becomes 1in

I believe that you mistakenly chose the first option, Same Dimensions so Pro/E did not convert the mm values into inch values. Instead it multiplied the models size by the conversion factor.

To fix you need to convert back to mm using Same Dims option.
Then convert units to inch again but select same size option.

Michael

 

[pamccrac]

Thanks Michael

I'm in wildfire 3...


I have some tools that have been created/added on in my drop down tool bar up top. one of them is "convert to inches" and another "convert to mm"

two questions
1) how do i do what you suggested without using these "shortcut macros"

2) how can i view these macros/add-ons and maybe even create my own

 

[mjcole]

Mmm French Bread Pizza yummy.

In Answer to your questions.

A1) Edit > Setup > Units
You will then see a menu showing different sets of units with a red arrow pointing to what the model is currently set to.

To change this double click on the row that contains the desired units and then select your choice of Same Size or Same Units and hit OK.

There may be issues with any parameters in your model not being changed such as a &THK parameter used in a relation to control a dimension i.e. &d0=THK will not get converted to the equivalent value during Unit Conversion.

A2) I would not suggest modifying your company macros.
However this can easily be done by going to Tools > Mapkeys selecting the macro and hitting Modify and Record. This will allow you to record a new sequence of Pro/E commands and then Hit Done and Save the modified mapkey.

Create your own Mapkeys hit New in the Mapkey dialog and then type in a letter code combination and description such as.
code Description
ecid Edit Convert part to In same Dimension
ecis Edit Convert part to In same Size
ecmd Edit Convert part to Mm same Dimension
ecms Edit Convert part to Mm same Size

Then hit record and go through the part conversion described in the description and hit Stop to finish the Mapkey and select Save All and enter a name for a personal mapkey file such as mymapkeys.pro and save it to your working directory. Or you can select save changed and save it to your personal config.pro file.

Michael

 

[mjcole]

You might want to check your Drawing Options setting for Dual Dimensions it may be set to secondary

 

[pamccrac]

all this was very helpful!
Thanks

 

[cadcamguy]

Mmm French Bread Pizza yummy.

and you're not sharing ... they are good aren't they