A while back I have posted a RAL appearance
library and it’s been copied, shared, and spread all over, some crediting while others not but you can still identify your own work
especially if you’ve done a mistake or two.
While
I don’t use it anymore I have been asked by colleagues on my previous company
to see if I can migrate, update it to work with 2015 and now with 2017 so I’ve
decided to share it once again for the greater good. Some people will take
credit, not doubt about it but that’s life and not why we are here.
Unfortunately
it didn’t quite migrate as expected and I am seeing the colors a lot brighter
in 2017 preview window almost as if they had self illumination, which I did check and it’s
not.
Don’t be fooled
by this, it’s only the preview thumbnails that have brighter aspects and the
models will look right, and so the edit appearance window.
Small mismatch
Use
it as it is, good or bad it’s still better than renaming an existing color manually
every time.
This
is especially useful in 2017 now that we can use the appearance as a reported property,
in parts lists, bom, notes, etc.
The model Appearance value is added as a selectable
property. You can add the Appearance property to a bill of materials, or a
parts list.
“
Appearance property
While I can send the library and provided a
detailed description on how to attach and use it, I feel it’s better if I just
give you a part with all the appearances locally and you can copy it to your preferred
library.
Don’t
you think so?
Almost forgot to share the link, that would have been useless ! Here is the 2017 part file.
In one of my previous post I’ve shown you how to
change length parameter format for steel shapes in Content Center (CC) so that
assembly Bill of Materials (BOM) will have no trailing zeros and round up the
value to a 1 mm increment.
On that post I gave you a bit of ilogic code that
can change formatting of files you might have generated already which can come
in hand and can be used with code injector.
At that time I didn’t realized that you might not
use the assembly BOM to report your lengths but use the drawing Parts List so
in this post we will look at doing just that.
If your company uses Parts Lists then you might be
lucky and saved yourself a good couple of day’s work where you needed to copy
all the default libraries to a custom read-write and then editing all the
templates to report correct length parameters.
The Parts Lists can be formatted just like the
parameter display and you can show/hide, trailing or leading zeros, units
string or even change units to: in, mm, cm, m, ft, yard, mi, or microns.
Double click on your table or right click and choose
“Edit Parts List...” either on the browser or graphical window.
Right click the quantity column and choose “Format
Column...”. In the format column window you can specify a new name for the
column, change text justification and most importantly you can change units formatting.
Click on “Apply Units Formatting” to activate the
submenus. Now you can change trailing or leading zeros, change units type, units
and precision. It can be configure to report a different measurement unit,
to change decimal from "." to "," and you can choose if you need to have
the units string displayed at all.
If you use the Materials List table style supplied with
Inventor you will have to modify the Substitution tab in the format cell window.
In the Substitution window you might have “Enable Value Substitution” and “When
exists, use value of” PL. This is helpful for those that do Tube and Pipe where
the reported parameter for pipe length is PL.
And of course there’s a catch. Your units will be
rounded but you need to be careful because you can have it rounded up or
rounded down. Both can cost you and rounding up an expensive material can be
just as expensive as rounding down and not having enough to complete your
design.
My settings will keep units to mm but will remove
trailing zeros and set precision to 0 decimals. Most workshops will not need or
manufacture to less than 1mm increments but this is for you to decide.
In this way you can keep the default formatting of
CC and keep working with the out of the box libraries without the hassle of
copying or editing them.
Today I'll show you my way of showing part info on dxf exported drawings. Every once in a while we do dxf profiles of flat pattern sheet metal parts and we need to add more info to each export. We don't always have time to do a drawing for each part but we add views of flat pattern parts on the main assembly layout (or in separate sheets) so we need the extra info on the views for the manufacturer.
We normally have: Part number, Material, Quantity, and Thickness as a note linked to each flat pattern view.
Here's how we do it:
1. First you need to expose the Thickness parameter of the model so go in functions (part environment) and mark "Export" box on Thickness. I would suggest you do this on the sheet metal template and maybe part template as well (in case you use the convert to sheet metal option).
This will add the thickness in custom iproperties of the part.
2. Create a drawing and add a view of a sheet metal part.
3. Add a custom symbol and in the sketch start a text with the following values:
Part Number: <PART NUMBER> link this to the model properties.
Material: <MATERIAL> link this to the model properties.
Finish the symbol creation for now.
4. Add custom part iproperties PJ_QTY :
4.(a) manually in the part properties
4.(b) In the BOM of the assembly. Open the BOM inside the main assembly (main project assembly) and go to parts only (you might need to enable it first). Click on add custom iproperties, type Thickness and type PJ_QTY (or whatever your want to call the part quantity). Add "Item Quantity" and have it next to PJ_QTY. Select the values on the Item Quantity and drag the lower corner of the last cell towards the PJ_QTY row just like in Excel. The PJ_QTY part properties gets created on all parts with the value from Item Quantity on it.
5. Go back to the drawing and place your symbol on an edge of your sheet metal part just like you would do with a balloon.
6. Edit the symbol, and the text in it. Because we linked it to a part with custom iproperties they are available to be referenced. Let's add the following text:
Quantity: <PJ_QTY> link this to the custom properties of the model.
Thickness: <THICKNESS> link it to the custom properties of the model as well.
7. Finish the symbol editing.
Now you can copy/insert it on any view, on any drawing before dxf export.
I would suggest that you copy it to the drawing template ready to drop in when needed.
Notes:
If you want to add Thickness to standard.ipt template you would be better to open it, convert it to sheet metal and back to normal. The parameters are part of it now and you can mark export on Thickness.
And the video:
In AIP 2015 that I am using now it exports fine but if the dxf export shows up <PART NUMBER> instead of the actual value you need to tweak your export options to convert Drawing Symbols to Blocks.
In the Save As dialog click Options, then click Next in the DXF Export Options and in the Export Destination window click on Mapping Options. In the General tab click Convert Drawing Symbols to Blocks. You can save the configuration for later reuse if you want.
If you need to explode the block in Autocad head over to Express Tools (this needs to be marked at installation it doesn't' come by default) and then use Explode Attributes rather than using the explode command.
In 2015 no matter of the settings in the save as options or the explode method it's working but in older versions I remember needing to take this steps.
