Altium Draftsman questions - Page 1
Forum section: electronics / general

author: Pack34
author_rank: Frequent Contributor
timestamp: March 09, 2017, 01:08:42 pm
content: I've been going through a variety of training to get comfortable with the software to make the switch from Eagle and I have a few questions regarding the proper use of the Draftsman tool.1. BOM inside the sheet? I see that there's a tool for this, but what would be the advantage of putting this in the draftsman document instead of just as a separate excel file? It just seems like another thing to keep updated.2. Title blocks. I'm not seeing an option for a title block in this. Is this something that needs to be manually generated?3. Dimensioning to centroids. When I provide dimension figures, I always provide a distance from a corner to center mass of a connector. The linear dimension tool seems to want to only snap to edges. Is it possible to dimension to centers?4. What should be included? To my knowledge, this is the document that would get submitted to the board house along with the standard quote packages. So what would be required would be:a. Dimensions from an origin to all of the critical pointsb. Layer stackupc. Manufacturing specification (material, plating, tolerances, finish, etc)d. Fabrication views. A listing of all of the gerber layers, drill drawing, and drill table.e. BOM?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 09, 2017, 10:13:49 pm
content: FYI, I don't know if this is specific to Draftsman or not, but:I usually place a cross on a mechanical layer of my footprints, to indicate centroid (or if not the centroid exactly, then a suitable datum based on the part shape or mfg drawing). This can then be measured by snapping the dimension to the shapes on that layer.If Draftsman works very differently from regular, then Idunno.Tim

author: ajb
author_rank: Super Contributor
timestamp: March 09, 2017, 10:36:48 pm
content: Re: BOM, it's an easy and quick way to generate a BOM, but not a replacement for a separate document. I wouldn't bother with it; an Excel file is much easier to deal with when it comes to actually using the BOM (both as the designer and as the purchaser or CM). Plus, unlike a draftsman BOM, an Excel file can be multiple pages. Nobody wants a BOM that needs to be printed on ANSI E to be legible.

author: pigrew
author_rank: Frequent Contributor
timestamp: March 18, 2017, 03:56:59 am
content: My company wants a PDF with pretty borders on ANSI specified paper sizes for the BOM table, so Draftsman would work well for that....However, there seems to be no way to add custom columns to the table (only the default columns like comment, footprint, etc), so no part number can be listed. Fail.

author: Mattylad
author_rank: Regular Contributor
timestamp: March 20, 2017, 12:24:40 pm
content: Although I have only had a brief look at this in my Altium, this looks exactly like Blueprint PCB from Downstream - I wonder if there was some integration?Quote from: Pack34 on March 09, 2017, 01:08:42 pmTraining is good, having a trainer to ask is betterQuoteThis is the point of tools like draftsman, it allows you to create the manufacturing\assembly package intelligently linked to your design file.If you have a separate excel spreadsheet then this has no link whatsoever to your design, change the design and the spreadsheet needs changing but is easily missed.The Draftsman document stays in sync with the design, so changes are implemented and you are far less to have them out of sync.Some people like the BOM on the assembly drawing, an essential document for all from assembly house through to the repair dept. (not really feasible on high component count boards)This is not a replacement for the BOM produced from Altium itself.QuoteWatch the video below, it includes templates - want something different then change the template.Open a draftsman template, edit it to have your preferred items on it - save it with a new name.QuoteIMO that tool is primarily to dimension the board, drilled holes etc. Not component locations.A corner? corners can move - you should be adding dimensions to a fixed location, such as an on board fiducial.On the assembly drawing, as above, add a figure on the component for the centre of mass, you can only snap to what is snap-able to - look at the document properties for this. See below for more on this.QuoteAs a master drawing for the fabrication this is good, ensure the dimensions are from a drilled hole and not the edge, dimension from the hole to the edge instead.You do not need to dimension components for the fabricator, just PCB items.The fabricators do not need a BOM.Your layer stackup must match what the can do - don't try to come up with something special unless your prepared to pay top dollar for it. (i.e. check with your fabricators before deciding on what stackup to use)Create a separate assembly drawing for the assemblers, this includes any critical assembly dimensions (not SMT placement) and the BOM if req'd. (although this is often a separate sheet in case values change but the assembly drawing does not need to). Mounting methods, assembly order, coatings etc.Component centroids are included in the centroid\pick n place file - this is then imported into the placement machine front end software for offline preparation of the job - do it using a drawing and its an awful lot of work and plenty of potential mistakes.Watchhttp://www.altium.com/video-intelligently-automate-your-documentationRead the documentation.@Pigrew: RMB on the BOM and go into the properties, on the Columns table click "Add", whatever std ones it adds, you can rename them. Look further at that.MattCID+Not a regular Altium user

author: mehmet.ali.anil
author_rank: Newbie
timestamp: March 20, 2017, 09:31:22 pm
content: I think, with a proper template that you agree upon with you manufacturer, Draftsman really puts schematic to the center of the design, and everything generated from that.QuoteIt really helps with the Assembly view, which you can relate to that particular component and take a note about it. (182 has 0.5 pitch)I believe it also helps to have all the assembly related parameters in one page. We have MSL, Pb-Free, etc as parameters in our library and you can just add a column for them.Given that, if anyone knows how to split the BOM into several pages, I will be very glad to know how.QuoteI have the attached for my PCB orders. (sorry, omitted design)And I append the stackup and my notes on impedances, all layers with my notes on specific points on those layers, and the drill drawing with the drill table.For assembly documentation, I just started working on that, I think one can include the assembly view and indicate THT parts, hand soldering, wave soldering, wave direction, specific visual checks to be made in between two processes. I would definitely mark where the thermal profiles are going to be taken, and with which profile parameters. Not fitted components shall be visible, Any data that might have been missed on your side but can be made visible during assembly counts. The form fields might have Optical Insepection Y/N, relevant stencil, quality control IPC class, requirements for the solder, lead-free and so on.

author: pigrew
author_rank: Frequent Contributor
timestamp: March 21, 2017, 12:29:46 am
content: Quote from: Mattylad on March 20, 2017, 12:24:40 pmI just checked the Altium bug tracker, and it seems that others have had trouble with BOM parameters, too. The trick ended up being to reconfigure Draftsman to use the "project" as the BOM source, instead of the "board" (which is the default). This choice is in the BOM configuration window.Sent from my HTC+10 using Tapatalk

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 21, 2017, 12:50:31 am
content: FYI, the same step is also necessary to activate project variants in the OutJob.Tim

author: SunnyDaze
author_rank: Newbie
timestamp: September 21, 2017, 01:01:36 am
content: QuoteTo see how to split the BOM in Altium Draftsmans, into mulitple tables, see the linkhttp://www.altium.com/documentation/17.1/display/ADES/((Draftsman))_AD, and scroll way down to that section.Here's what it looks like:

author: SunnyDaze
author_rank: Newbie
timestamp: September 21, 2017, 01:17:24 am
content: Quote from: Pack34 on March 09, 2017, 01:08:42 pmMy employer requires a "Parts List" on the first page of the drawing, and the Draftsman linked BOM works better for this than anything.QuoteThis is part of the template. We have our own templates, and have pointed Altium to that directory, so they show up as default templates.QuoteNo. don't see that option.QuoteThe gerber file gives the board houses all the dimensions necessary to build the PCB, and the drawing tells them how to put it together. On my drawings I provide:BOMFabrication Notes across the pages. Draftsman will split the Notes across the pages, and keep them in numerical order throughout the document.Board Assembly views, at least Top & Bottom.Drill TableDrill Drawing View (w/all the necessary dimensioning attached to it)Layer Stack-Up LegendFabrication Layers- Top & Bottom Copper/Solder, Internal Copper Layers, Top & Bottom Solder Mask, Top & Bottom Overlay Silkscreen, Top & Bottom PasteAnd then I create an OutJob and attach the schematics to the drawing as the last pages.This all goes together very fast if you put the right parameters in your schematic library, and/or in your parts on your schematic to begin with. I can whip out a peer-review ready drawing in half a day using Draftsman if the parts are all set up to begin with.