@ltium - A few question

EDAboard.com Forum Index -> PCB Routing & Schematic Layout software & Simulation

Author

Message

Dotnet

Joined: 02 Jan 2008
Posts: 6

03 Jan 2008 0:22 @ltium - A few question

Hello All

As @ltium doesn't have a library entry fot the Holtek 12E (or family) what are you supposed to do when wanting to enter a circuit?

I'm trying to use a generic DIL-18 entry (from PcbLib) to allow me to enter my circuit shematic so that I am able to autoroute with ground planes etc. - NO!! If a SPICE listing for these were available then I would invest the time (and learning curve) creating a new component - obviously without SPICE I can't simulate but surely you can enter a circuit without using simulation?

How can you import DXF files without @ltium thinking the lines are tracks and giving them thicknesses - I need the imported lines still to be boundaries so that I can fill them with copper to form contacts for a PCB based rotary switch. (to use a third parties enclosure)

How can you fill a round shape with copper - is there something like a bucket fill option as in photoshop?

What little hair I have left is coming out - any help would be appreciated

Cheers
Matt

House_Cat

Joined: 21 Feb 2002
Posts: 1330
Helped: 274

03 Jan 2008 1:23 Re: @ltium - A few question

There are very easy-to-use library editors for both PCB footprints and schematic symbols. If the included libraries don't have what you want, it only takes a couple of minutes to make a footprint or symbol. The Holtek 12E series are small 18-20 pin devices - it would take very little time to make schematic symbols. PCB footprints are standard packages, so they're already available in the libraries.

Yes, you can enter a schematic symbol or PCB footprint without a simulation model. I don't understand what problem you are trying to report.

If you are going to use the DXF import to make a solid copper area, it doesn't matter if the lines are imported as tracks. If you set your clearance design rule to "0", or delete it, you can pour copper to the centerline of the track (which is the same as the centerline of the imported DXF line). You can also give the boundary tracks and the polygon a dummy net name, then tell the software to "pour over same net objects". Additionally, if you want the imported line to have a smaller width, there is a box in the DXF/DWG import dialog that lets you select the default line width.

To pour a polygon using a predefined boundary, you first select the boundary. You then go to menu item "Tools>Polygon Pours>Define from Selected Objects". This function is only available starting with version 6.8. If you are trying to use an older version of the software, the procedure is a bit more complicated. Let me know what version of the software you are trying to use if you aren't using the latest.

It sounds from your questions like you may be in over your head. A professional EDA package like @ltium Designer is not intended for casual use. It is feature rich, and takes time to learn. Unless you are willing to put in the time to learn the tool, you may want to start with a simpler tool. @ltium Designer, PADS, Allegro, etc. are professional/semi-professional design suites. Eagle, by Cadsoft, is a popular low cost package that is easier to learn for beginners. You will still need to learn how to make your own schematic symbols and PCB footprints.

Dotnet

Joined: 02 Jan 2008
Posts: 6

04 Jan 2008 0:28 Re: @ltium - A few question

Hi House_Cat

Thank you for your reply.

It certainly sounds, to say the least, as if I have had my wrists and knuckles slapped by your reply!!!

I'm getting back into Electronics after 20 years and I'm looking at packages to 'hold my hand' at the design stage. Some people waste their money on fast cars I'm looking to pick up my HNC electronic engineering and invest in my knowledge and in something which I enjoy. Yes the product is completely different to the software I trained with which ran on 386DX 128Mb RAM, but these days I find there's very little info out there to help (remember Maplin catalogues semiconductor section?)

I am currently running an evaluation pack v6.8 from @ltium

I do agree - to a point - that I am over my head but it's more with terminology of the program and working out what the software expects from me which is the same for any package. I was completely perplexed by my wife's copy of Photoshop until she explained the concepts of the layers.

So I apologise for asking a question on your forum, especially when it was late, when I was frustrated and @ltium's technical support were closed.

Matt

House_Cat

Joined: 21 Feb 2002
Posts: 1330
Helped: 274

04 Jan 2008 3:14 Re: @ltium - A few question

No slap intended. I was only trying to suggest a simpler alternative. Professional tools like @ltium Designer, Mentor PADS, and Cadence Concept/Allegro don't hold your hand. You either know them or you don't, and acquiring skill is a long, hard, process.

@ltium Designer has a steep learning curve. The company runs training sessions, but there's no tutorial available to lead you through the software step-by-step. The "Help" sub-directory of your installation has numerous publications covering every aspect of the software. In addition, hitting the "f1" key while hovering over a menu item will bring up help documentation on-screen. Hitting the "~" key while performing a specific function, such as placing a track, will bring up a menu of available keyboard shortcuts affecting that function. The "Knowledge Center" available from the menu bar "Help" function, or from the help button at the lower right of your screen brings up a search engine to find information in those documents I mentioned earlier that are in the "Help" sub-directory.

Dotnet

Joined: 02 Jan 2008
Posts: 6

10 Jan 2008 0:48 Re: @ltium - A few question

Hi House_Cat

Yeah! fair point there are easier packages around.

You obviously have been in the trade for a fair few years and no doubt you know where I'm coming from when one is being 'beaten' by a problem - especially electronic engineers they do there damndest (spelling) to solve it.
I have been self employed in the IT business and Server market (both hard/soft ware) I now my around software but @ltium is/was beating me, there just seems no logic to it - it's frustrating!! I'm just used to a hierarchical type of software not horizontal I suppose. (old dog......)

Gone are the days of the good ol' Z80 and stripboard (lovely capacitance!!!) eh!

I am going to persevere with @ltium for a while - just for personal satisfaction before it gets uninstalled so I apologise in advance any overly a*al questions.

Cheers House_Cat
Matt

Last edited by Dotnet on 10 Jan 2008 16:22; edited 1 time in total

House_Cat

Joined: 21 Feb 2002
Posts: 1330
Helped: 274

10 Jan 2008 3:50 Re: @ltium - A few question

Keep the questions coming. I'll try to answer them.

Altium Designer is a beautifully integrated package, and there is logic. It just takes a while to learn it. The features in AD are mostly the result of user input and are evolving constantly. Every update to the software has new features in addition to bug fixes.

It is hierarchical, you define a project (PCB, FPGA, Scripting, CAM, etc, and you choose project options that you want for paramters, net scope, electrical rule checking, etc. If it's a PCB project, you then develop the project libraries of symbols and footprints by either copying from the provided libraries or your own creations, which you then put into your schematic which can be flat or hierarchical. The schematic is then "compiled" which is really their terminolgy for doing the ERC (electrical rules checking), and extracting the netlist. You then export the compiled schematic to the PCB document, and the footprints are dumped for you to place manually, or autoplace. From there you add any design rules (constraints) you want for the PCB, and you either manually route or autoroute. Design rule checking can be done online continuously or in batch as the board develops. Simulation of the circuit can be done if you have delevoped the PSPICE models for your design or taken them from those provided in the Altium provided libraries. You can cross probe from schematic to PCB or vice-versa to check your circuit manually. Finally, you can output CAM files in Gerber or ODB++ format, and check them in the integrated CAM editor (Camtastic). All of the documentation can be done from one location - the Outjob File. You can set it up to output to any device, including PDF, and it has entries for schematic, PCB plots, fabrication files, Gerber files, Drill Files, test point reports, IPC netlists, ODB++, simulation results, BOM, etc. Once you set up the Outjob File, you never have to set up the output formats you want again.

So the hierarchicy goes like this - Project>Project Rules and Settings>Libraries>Schematic with PCB Directives>PCB with extended design rules>Design Rule Checking>Simulation>Outjob for documentation and fabrication>CAM file verification.

You can get some sense of the flow and flexibility of the tool from going to the Help menu and selecting "Getting Started". The PDF documents are listed in a logical order to lead you through the early stages of learning.

fala

Joined: 18 Sep 2005
Posts: 246
Helped: 15

10 Jan 2008 9:03 Re: @ltium - A few question

Hello Dotnet:
while House_Cat is right and there are easier packages, but First of all I think there is nothing wrong if you want to work with @ltium designer or even allegro(which is even more difficult). As you very rightfully said some people spend their money/time on fast cars but it is yourtime and money so spend it whatever you enjoy it the most. Actually I think AD is very attractive to beginners because of its 3d features absent in other packages that I know.
Second of all I think you do not need to master Altium to work with it (even professionally). I work with altium designer for more that 3 years(not full time of course) but I have to confess I'm not master of it. it has many features that I'm not familiar with(because I never needed them) but I work professionally with it and I earn good money. So you can start it in basic form just draw schematics-> place component-> auto rote/manual route it-> generate gerber -> sell your board. over time you gradually feel the need to learn more about other features. for example PSPICE simulation or when you work with high speed/ long tracks signal integrity checks,.... and you will learn those features when you needed them.
Third of all people here are very friendly and helpful especially House_Cat who is a real master in AD and in layout in general is extremely helpful and good-tempered.
so you are welcome here to ask your questions.
cheers

Dotnet

Joined: 02 Jan 2008
Posts: 6

10 Jan 2008 16:09 Re: @ltium - A few question

Hi Fala

I REALLY do appreciate you post - thank you.

O.K. then I wonder if you could point me in the right direction with what I am working on. The project is using a third parties RF transmitter remote control enclosure which allows the address of the transmitted data to be altered via an on-board (custom) BCD Rotary switch

I have uploaded two BMP's direct from ACAD (via Paint) one is a full outline and the other is an enlarged view on the rotary wiper track I'm trying to recreate. What I haven't included is the four tracks from this matrix to the encoder.

White lines board outline
Red circles 1mm through holes for Switches (ultimately pads)
Yellow are holes in board to lock and locate switch mechanism & plastic cover (critical placement)
Blue circles are 2mm holes for battery connectors
Green lines BCD Rotary switch layout (critical dimensions)
These are all on separate layers in ACAD!

Now, I obviously will be importing this over as a DWG or DXF then what?
Which layers do I specify in @ltium for each area I have created?
How do I get the green areas filled with copper using the green lines as boundaries?.
How do I specify the red and blue holes are to be connected (with exact dimensions) into @ltium? I don't necessarily care about the size of final pads but the X,Y coords of the holes are VERY important to align with the third parties switches in the outer case.

Cheers
Matt

Sorry, but you need login in to view this attachment

Dotnet

Joined: 02 Jan 2008
Posts: 6

10 Jan 2008 16:33 Re: @ltium - A few question

Hi House_Cat

Sorry, I missed your reply (before Fala) to my last post - it makes things a little clearer.

The area I was going wrong (possibly) was that I have very rigid constraints to my circuit board, I was trying to set thoses constrains before th schematic was in place assuming because the package seemed 'flat' it could deal with those criteria.

Subsequently, you previuos comments on component footprints now seem to make more sense.

So, let me get this straight, you set up all the components anticipated BEFORE starting the schamatic?

But I again reitterate a previuos question how can I place a generic 18-pin DIP into the schematic so that I can finish the schematic and subsequently produce a net

Also, what Altiums meaning of 'ROOMS'

Thanks again
Matt

fala

Joined: 18 Sep 2005
Posts: 246
Helped: 15

10 Jan 2008 17:43 @ltium - A few question

Hi Dotnet,
Ok When you import a file from autocad a dialog appears, you can specify your insert location and how to convert autocad units to AD units there. you will define each auto cad unit is how many mills and you define insert location(refrence points are Autocad origin and AD origin, you can change AD origin Edit>>origin>>Set). if your drawing is in different autocad layers each layer will be inserted in a different layer. Now you have two choices use this component once or insert it as a PCB library component so you can use it whenever you want without having to import the drawing each time. First solution is easy second may have a little more difficulties but it will be a great relief if you occasionally need this component. For first solution just select ALL the lines(press SHIFT) that you want to be connected to a net and then open properties(right click) , PCB inspectors open so you can change properties of all of them at once. then you can change their layer(presumably to top layer and specify the net that they all should be connected to( both are available in their respective combo box).
For second option you have to create a schematic and a pcb library. in schematic library draw the schematics and specify pin numbers. and in PCB library(copy-paste the lines you imported in your PCB). I don't know a way directly import Autocad to library maybe House_Cat knows. then you have to place pads in place of circles you created to represent pads(I forgot to mention in PCB you also have to do this). for placing copper fills.I don't know a clean way again maybe House_Cat knows but you can define the oulines of your copper fill as Keep-Out layer. place a pad or a track that has the same net property as your copper fill inside those outlines then place a polygon that encloses those outlines and select Pour over all same net objects and select remove dead copper and after polygon has been built only area inside keepout track outlines will be filled with copper(again you have to do this in PCB too, if you don't want to build a library). then for your schematic to be associated to the footprint you just created. open its properties in schematic library and add footprint and refer to the pcb lib you created. then you can easily place the part in schematic and automatically the footprint will be inserted in your PCB.
hope that helps. cheers

Added:
For another question regarding how to place a ganeric component. I think you have to create the schematic representation of it in your custom schematic library then you can associated with footprints already available in AD(use Add...>>FootPrint in property browse AD PCB libs you can find most standard footprints there)

Rooms are created to enclose a group of parts so you can place them more easily. you can move a room and all associated components will move together or you can select Tools>.component placement>>arrange within room so all scattered components be arranged in that room.

House_Cat

Joined: 21 Feb 2002
Posts: 1330
Helped: 274

11 Jan 2008 2:32 Re: @ltium - A few question

You can either make your schematic library before you start the schematic, or in parallel with the schematic development. I generally do as much library work as I can before I start. That way, I don't get impatient with myself when I want to place a symbol and find that I have to take time out to make one.

To add to fala's posting. You can't import DXF or DWG files directly into the library editor, you should do your import into a "scratch" PCB file, then copy the results into a library component. You definitly want to stick with drawing files to preserve the dimensions. Graphic files such as BMP can be imported by AD, but there is no guarantee of dimension with graphic files - in fact, the newer version of AD permits dynamic scaling of imported graphics at the time they are imported.

If I were doing the component, I wouldn't try to convert the circles to pads. I would identify the spacing, and the center of one of the circles. I would then set the origin temporarily to the center of the reference circle, set the grid to the spacing between them, and then just place the pads. The circles could be moved to a mechanical layer and used to verify the centers after placement of the pads.

The switch contact can be done as fala suggests. There's also a way of pouring a polygon into a selected boundary. If the demo you are using is version 6.8, there's a menu option in Tools>>Polygon Pours>>Define from Selected. Once again, you would do this work on a scratch PCB, then copy the results to the library component.

I would love a chance to play with your component footprint. If you're willing, you could zip and post the autocad DXF file. I would return the result of my effort as a library footprint.

jazzz

Joined: 21 Oct 2006
Posts: 42
Location: EU

14 Jan 2008 11:44 Re: @ltium - A few question

There is a way to edit power simbol in the AD6? Or to create the new ones.
For example, I want to create much smaller schematic symbols for GND.
Thx.

House_Cat

Joined: 21 Feb 2002
Posts: 1330
Helped: 274

14 Jan 2008 20:50 Re: @ltium - A few question

jazzz wrote:

There is a way to edit power simbol in the AD6? Or to create the new ones.
For example, I want to create much smaller schematic symbols for GND.
Thx.

You can't edit the existing power symbols in AD - they are system symbols. You can make new library symbols for yourself using the schematic library editor, and use them the way you would any other schematic symbol.

Dotnet

Joined: 02 Jan 2008
Posts: 6

14 Jan 2008 21:58 Re: @ltium - A few question

Hi House_Cat

I'm Back........(note to self - move MoT away from Christmas in future !!!!!!)

No problem with posting - do you want it private or public?

Just to aide my understanding - you're saying the outline of the switch contacts would become a component - why?

I have tried the ...........'define from selected' as mentioned in your earlier reply but the fill I ended up with did not fill to the boundaries it, sort of, Offset (autocad) the boundary lines (internally) and looked like tracks not fills. I obviously need to 'tweak' a setting - any suggestions?

Lastly, I've not included the 4 connection points to the encoder from the switch contact. Whaen the fill takes place I take it that it will be easy enough to add these tracks?

Cheers
Matt

House_Cat

Joined: 21 Feb 2002
Posts: 1330
Helped: 274

14 Jan 2008 22:31 Re: @ltium - A few question

You can either PM the file to me or post it - I'm just curious to see what I can do with it.

My suggestion to make the switch assembly a component is to lock down all of the primitives to avoid any changes in the relationship between the elements. Additionally, it will be necessary to include solder mask opening for the fill used to create the switch contacts. Without the manually placed solder mask, a mask layer covering would be generated in the Gerber files for the board. It's easier to make sure all that stuff is taken care of when locked into a component.

On your "scratch" PCB, try setting the clearance design rule to zero mils, or simply turn it off. That way the polygon fill will extend to the centerline of the boundary lines. The fill will, indeed, be represented by straight line segments as it follows the curves; however, it should be possible to keep the approximations negligibly small. One trick is to pour a polygon with the arc approximation setting at 0.0001mils (it's not supposed to be possible, but the internal resolution of AD allows it).

If you are getting what looks like a track instead of a fill, it's because of the settings for the polygon pour. You need to double click on the center of the fill area, bring up the polygon dialog, and set the polygon to "pour over all same net objects".

The final component can be connected with tracks that lead to any copper area. One thing to keep in mind is that any reference to "pins" on a schematic will have to include the matching pins on the PCB footprint. If you plan to represent the switch on the schematic, you'll have to give it identifiable pins that match the PCB footprint. That is done using the "pad" primitive. In your case, those pads will most likely be surface pads placed in the switch component at the appropriate locations for your track ends to connect with.

jazzz

Joined: 21 Oct 2006
Posts: 42
Location: EU

17 Jan 2008 0:23 Re: @ltium - A few question

House_Cat wrote:

Thanks for the reply.
Could you be more specific, please. Because I didn't know how to edit the existing library, I create a new one. Like common libraries. And because of that, when I place more than one symbol (the created GND) in schematics, it appears an error like in the image.

So I'll be very happy to find the editing procedure.

Thanks again. jazzz

House_Cat

Joined: 21 Feb 2002
Posts: 1330
Helped: 274

17 Jan 2008 1:05 Re: @ltium - A few question

jazzz wrote:

Because you have defined a new symbol with a pin, you also need to assign a net name to the pin. The error is just warning you that the pin is unconnected. Use Place>Net Label(shortcut PN), hit "Tab" before you place the label, and type in the proper net name. Place the label on the pin such that you see the red connection "X". You can't place a net label in the library, so it has to be done once your symbol is placed in the schematic.

If you are going to place a lot of the symbols, you can use "rubber stamp" to duplicate one of them. Just highlight the symbol and net label, then hit CTRL-R.

jazzz

Joined: 21 Oct 2006
Posts: 42
Location: EU

18 Mar 2008 0:32 Re: @ltium - A few question

Hi. I need your expertise, please.
I want to draw the track below to replace an inductor. I mean, the inductor will be represented by the track itself.
The question is, does AD have a tool that allow me to calculate the inductance of the created track?

Many thanks!

PS: There is a complete trainning manual of AD?

House_Cat

Joined: 21 Feb 2002
Posts: 1330
Helped: 274

18 Mar 2008 23:23 Re: @ltium - A few question

jazzz wrote:

I want to draw the track below to replace an inductor. I mean, the inductor will be represented by the track itself.
The question is, does AD have a tool that allow me to calculate the inductance of the created track?
PS: There is a complete trainning manual of AD?

Unfortunately, AD does not have a tool to calculate the inductance of your structure. Normally, a structure like yours would be created a 3D simulation program, exported as a Gerber or DXF file, and then imported to AD.

The training manual for the latest version of AD is available online at: http://www.@ltium.com/Community/Support/TrainingManuals/

jazzz

Joined: 21 Oct 2006
Posts: 42
Location: EU

19 Mar 2008 17:23 Re: @ltium - A few question

House_Cat wrote:

Do you know such a 3D simulation program?
Many thanks.

House_Cat

Joined: 21 Feb 2002
Posts: 1330
Helped: 274

21 Mar 2008 23:40 Re: @ltium - A few question

Unfortunately, 3D simulators are expensive. Two that I know are capable of doing what you want, and giving accurate results, are:

http://www.ansoft.com/products/em/maxwell/
http://www.sonnetusa.com/

jazzz

Joined: 21 Oct 2006
Posts: 42
Location: EU

21 May 2008 23:31 Re: @ltium - A few question

Once again I need your help, because I have to generate gerber files from a pcb project. So, my pcb looks like this:
- components are on both sides: THT on top layer and some SMD on bottom layer;
- the copper trace is only on bottom layer (single side).
In this tutorial you can see the next image

.
My questions are:
1. what layers do I have to check for my pcb?
2. do I have to check mirror for some layers (for example, bottom overlay) or just follow the steps?

House_Cat

Joined: 21 Feb 2002
Posts: 1330
Helped: 274

22 May 2008 2:54 Re: @ltium - A few question

No, you shouldn't check mirror. Gerber plots are meant to be read from the top down - just like your PCB editor shows the board. The Mirror ability is there for those who want to etch their own boards, or the odd fab who uses very, very, old equipment.

If you press the button at the bottom of the display for "Plot Layers", you'll see a choice for "Used Layers" - click on that and the appropriate layers will be checked for you.

Depending on what you want for your finished board, you may not use all the Gerber layers. For example, if you choose not to have a top silkscreen, you just ignore that Gerber plot.

jazzz

Joined: 21 Oct 2006
Posts: 42
Location: EU

24 May 2008 11:02 Re: @ltium - A few question

Many thanks, House_Cat

Because I have no experience of using gerbers files ans industrial pcb manufacturing, I need your advice, please.

This image represents the normal view in the generated bottom overlay gerber data? I mean the mirror comment is ok?
Can you tell me some other tricks of using gerber data, please.
It helps a lot avoiding heart failure Neutral

jazzz

Joined: 21 Oct 2006
Posts: 42
Location: EU

27 Jun 2008 19:13 Re: @ltium - A few question

How do I set 70 micron copper thickness in AD?
Thx

House_Cat

Joined: 21 Feb 2002
Posts: 1330
Helped: 274

27 Jun 2008 20:51 Re: @ltium - A few question

You set copper thickness by using a fabrication note, and a stackup diagram. Usually such notes and diagrams are placed on the Drill Drawing, but any mechanical layer can be used. This is the same will all EDA software. You need to provide a diagram and/or notes for the fab.

Copper thickness can be entered in the Layer Stack Manager (Design>>Layer Stack Manager), by double clicking on the desired layer in the diagram. However, that information will not be included in your fab files unless you place a stackup diagram (Tools>>Layer Stackup Legend) on a mechanical layer as I mentioned in the first paragraph.

jazzz

Joined: 21 Oct 2006
Posts: 42
Location: EU

05 Aug 2008 15:14 Re: @ltium - A few question

Hi,
My goal is to design a board with metallized pads like these ones

But I'm confused about the correct settings in ADS08, concerning the pad shape. Any help, please.

House_Cat

Joined: 21 Feb 2002
Posts: 1330
Helped: 274

05 Aug 2008 21:19 Re: @ltium - A few question

Unless I'm not seeing the picture properly, the pads that you're showing are simple plated-thru round pads. When building the footprint, you would just use the hotkeys "PP" (for place pad), hit tab to open the properties, and enter the information about hole size, pad size, plating, shape, etc.

EDAboard.com Forum Index -> PCB Routing & Schematic Layout software & Simulation

Page 1 of 1

All times are GMT + 2 Hours

Abuse
Administrator
Moderators

sitemap