Via/Pad holes in Cadstar?

[mkw]

cadstar n.c drill

Hi...
Please, i would like to know if is possible to print the via/pad holes in Cadstar 5.0?
When i print the routed layers (top/bottom) using Cadstar Postproccess the pads and via holes are filled with black color, wich is impossible to view the holes.
See picture on:
www.mkw.kit.net/sec2/cadstar.jpg
How to solve this?
Thanks.
MKW

 

[crypted]

drill holes in artwork cadstar

My problem is completely same with yours. But i use POWERPCB. By the way i haven't found any information about it.
good luck

 

[stefk]

create an nc drill output cadstar

Hi,
I think that is not possible inside Cadstar, but maybe if you use any third party post process tools (Gerber Tools for example) you could solve your problem .

 

[btbass]

cadstar nc drill

One way to do it is to turn all your pads into annulus, then you can print holes in the pads. I know what you mean, drilling a prototype board with out a guide is a pain in the arse.
:evil:

 

[mkw]

hole in a pad cadstart

Thanks to all for replies, i will try the btbass tip.

============================================
Hey crypted...
What is a version of Power PCB that you are using? If your version is 5.0 is possible to print the holes.(On version 4 i don´t know).
If you have the version 5.0, left click on pad to select , them right click on selected pad and choose Query/Modify, click on Pad Stack Button, select the 3 objects as show here **broken link removed** ; the value 25 is the size of hole that you need and you can change this value to more or less.
Note: For each different footprint that have on your design you need to select one pad of each different footprint. For example, if your design have one DIP16, one R1/4w and one DIP32 you need to select one pad of each item (holding control button) and clicking with left mouse button, on this case, using the three components above, you will need to select only three pads; but, if your design have one DIP16, ten R1/4w, one DIP32 footprints, you will need to select only 3 pads , because that design have 12 footprints, but only 3 different footprints.
When asked if you want to apply the changes for all pads, answer ALL.

If you have not understand, please contact-me for more informations.
MKW.

 

[cyberrat]

hole in a cadstar pad

As has been mentioned, you can:

Create a RS-274-X Gerber file of the copper layer.
create a drill layer.
Open them up in gc-prevue (free) and with the drill layer above the
copper layer (using A01 not Ro1), turn it to be composite and using
ctrl-d make negative layers black.

a quick adjustment of the hole sizes should enable you to print the
1 layers out, with holes in the pads.

(if you can get GC-Cam or cam350 etc its better for this).

However, if you do not have that many pads it may be easier just to change them to anuluses as said above.

 

[mkw]

cadstar help

Hi Cyberrat..
Thanks for your tip, but how to create RS-274-X Gerber file and drill layer?
Thanks.

 

[cyberrat]

gc preview change view holes

To create the GErber files, change your colours,layers and whatever is viewed to only be the copper layer. I.E. bottom copper.

Then from the main menu, select File, Manufacturing Export, Artwork.
In "Setup Device", choose "photoplotter" and then "Setup" browse to your \User\RS274-X.usr file and OK.
(output to file too)

Choose "Scale and position" and ensure that it it 1:1 and fits on your bed.

Then the "Start Processing" button will enable you to select a path/filename and start the plotting.
This produces the copper layer Gerber.

To produce the NC drill data, from the manufacturing export choose "NC Drill".
Setup the device to be NC Drill & Excellon.usr.
Check scale etc.
In OPtions, chooses plated through holes or not, perhaps you may need to do both files.
Tick "Drill optimisation".
OK and create the file.
Note, if you also do a non plated drill file, the drill tools will start from "1" and may be of a different size to the plated through hole tools.

Hurridly written, but I hope it helps you in looking at how to create Gerber files.

Roland.

 

[przem188]

cadstar gerber

**broken link removed**

 

[antarveena1982]

cadstar to pads

Hi MKW


I am ageeing wiht Cyberat you have to make gerber file and use CAM software to visualize holes and if you have powerplaane layer tahn you have to see negative of that.

Hope this will help you.

regards
Antarveena

 

[CC1111]

print drill cadstar

I would like to know if sizes indicated in gerber drill files generated by CADSTAR are tool sizes or finished hole sizes.

Best regards,
CC1111

 

[Mattylad]

manually create via cadstar

The sizes in the NC drill files are whatever you setup in your assignments and are dependant upon how you work & provide data top a PCB fab house.

It is usual to setup your pads to drill at the finished size that you expect the hole to be and your fab house will adjust all the sizes at their end to do this.

I.E. if you want a 0.8mm hole, they may drill at 0.9mm when they are expecting 0.1mm of plating thickness, so you set your hole to be 0.8mm.

When generating the drill files do not use Gerber you use excellon output and if available the excellon2.usr file which embeds the drill sizes in the files (equivalent to RS274-X extended Gerbers but for drilling).

If in doubt use the help files and the self teach training files to give you a good grounding on manufacturing output.