Notice. New forum software under development. It's going to miss a few functions and look a bit ugly for a while, but I'm working on it full time now as the old forum was too unstable. Couple days, all good. If you notice any issues, please contact me.
|
Forum Index : Microcontroller and PC projects : Sprint Layout 6.0
Page 1 of 4 | |||||
Author | Message | ||||
Rickard5 Guru Joined: 31/03/2022 Location: United StatesPosts: 328 |
I was going to post this in the PCB SUB, but the newest post there is a year old, so I hope it's ok I posted here . I got Sprint Layout 6.0 a few weeks ago because I know some of you guys use it, But even though it's looking easy to figure out, the documentation does leave something to be desired, and I have some questions Just to start off with, 1. on 2 layer board board when I place a part, will that place a solder pad on both top and bottom? will it automatically plate though the board, so when I solder a part on the bottom of the and get a good connection to a Track on the top side of the board? 2. How do I draw Board shapes and add AC Isolation Slots?, I'm trying to make custom shaped boards for robots Thank you for any Info Rick I turned the volume on the monitor to max and could hear sound. Thanks Stanleyella |
||||
Mixtel90 Guru Joined: 05/10/2019 Location: United KingdomPosts: 5648 |
1. It depends on how the item was saved. You might find that some items are saved with the pads on the bottom layer only - it's easy enough to make them plated through pads. There's a box to tick when you highlight the item. I use the second smallest round pads as vias. You can also highlight individual pads or parts of an object by holding down Alt while you click on the bit you want. This allows you to do things like deleting pads & stretching outlines to make odd sized connectors. 2. There is no slot command. You have to put a row of chain drilled holes on layer O to get a slot. Boards are always rectangular by default but you can warp them. e.g. draw a rectangular outline on layer O. Now highlight it and you can see the corner nodes and mid-point nodes. You can stretch the mid-points out of position, creating new mid-point nodes on each side as the new position becomes a new node. It's easier to do than to explain. lol. You can have as many nodes as you want AFAIK so the system is quite flexible. You can't have true curved PCBs though AFAIK. (Incidentally, it's probably better to change the grid to 1mm when messing with the board outlines. That way you end up with true metric sized boards with sensible fixing centres - unlike your horrible US decimal inch system. ;) More seriously, it makes sense if you want 100mm square PCBs for JLCPCB.) Edited 2022-09-24 20:30 by Mixtel90 Mick Zilog Inside! nascom.info for Nascom & Gemini Preliminary MMBasic docs & my PCB designs |
||||
Tinine Guru Joined: 30/03/2016 Location: United KingdomPosts: 1646 |
L6 is sooo intuitive that the built-in help is really all you need. Wonderful piece of software. Like anything else, you need time but man, this thing puts a smile on my face. I would rate this 20/10 Craig |
||||
Grogster Admin Group Joined: 31/12/2012 Location: New ZealandPosts: 9030 |
F12 will change any highlighted footprint from single-layer, to two-sided with plated through holes. So, click a part, and press F12. The pads will change from green or blue, to light blue, which means it is a plated-through pad on both sides.(when using the standard colour scheme) Basically, you are turning the pads into vias, but just all pads in one keypress for any pre-defined component you have placed. Repeat to turn the pads back to single-layer if needed. If you have enabled ground-planes on your top and bottom copper layers, F12 will space the pads off the ground-plane on both sides. STANDARD vias I let the factory cover in soldermask. My standard size for most signal tracks is 0.2mm with 0.4mm space between track and any ground-plane(default), a 0.3mm hole with 0.7mm pad size. Use the pad tool, place a pad, adjust its size to 0.3/0.7, click it to select it then press F12 to make it a through-hole via, then click on the SOLDERMASK tool, then click on the via you just made, then click on EDIT again. From that point, you can then copy that one via to as many places as you want(right-click the via, select DUPLICATE), and they will all be the same size, and covered in soldermask. This can save you a HUGE amount of time, if you have to "Cover" them all with soldermask manually later, as you could have lots and lots of vias. Further to what Mick said, making LARGE holes or cutouts in your board, is done by drawing the shape on layer zero. If you wanted a 30mm hole in your board for a huge arcade-style button for example, you draw a circle with the circle tool, on layer zero. EDIT: VERY quick example of a 6-pin DIL opto-isolator with a slot cut underneath it. This is a 0.635mm grid, so the slot is 3.8mm wide. Note the light-blue pads on the opto, meaning this part has plate-through holes, with pads on both top and bottom of the PCB. A tool I particularly love, is the photoview tool, which is like a cheaper version of the 3D view that some more exotic CAD software can do. This just lets you see what your board will look like as you go. The one above looks like this: Edited 2022-09-24 22:55 by Grogster Smoke makes things work. When the smoke gets out, it stops! |
||||
Grogster Admin Group Joined: 31/12/2012 Location: New ZealandPosts: 9030 |
You can, but it requires much more work then standard square or rectangular. To make a curvy board, I start with the CIRCLE tool, and draw a circle of suitable size. Click the circle, drag the node to turn the circle into an arc. Right-click/Duplicate as needed. Flip H and V and rotate as needed. Place till you have the final outline. Use the track tool to draw lines between the nodes on the arcs. Smoke makes things work. When the smoke gets out, it stops! |
||||
Mixtel90 Guru Joined: 05/10/2019 Location: United KingdomPosts: 5648 |
Silly me - I've done cutouts with rounded corners the same way. lol As long as the outlines are on layer O you are fine. I usually put a roughly drawn X inside cutout areas just to clarify - it seems to have worked so far. :) If you are using headers or SIP connectors from the standard library check the hole diameters! They are 0.72mm by default, which is no use for any of the male header pins that I've tried. You need to change them to 0.8mm or even 0.9mm. Just a couple of points - if you are using JLCPCB anyway: They might charge extra for rounded corners as they mill them out rather than guillotine. In some cases they do it by hand, so the cost goes up even further. I've not fallen into this trap yet, but no guarantees. Don't be tempted to put more than one design onto a 100mm x 100mm pcb to try to get several done cheap. You are charged per design, not per board. Also, the cheap offer doesn't include V grooving - you have to cut your own boards up. Mick Zilog Inside! nascom.info for Nascom & Gemini Preliminary MMBasic docs & my PCB designs |
||||
Rickard5 Guru Joined: 31/03/2022 Location: United StatesPosts: 328 |
Ohh you're talking about Imperial? didn't we inherit that from our British Masters? after Whitworth I guess even the French could do a better job! ohh so how's that EU Common Market thing going? :) please don't take offense, I'm Joking well except about stupid Whitworth I turned the volume on the monitor to max and could hear sound. Thanks Stanleyella |
||||
Tinine Guru Joined: 30/03/2016 Location: United KingdomPosts: 1646 |
Pass me the thirteen sixty-fourths wrench Craig |
||||
Mixtel90 Guru Joined: 05/10/2019 Location: United KingdomPosts: 5648 |
We find it difficult to find a ruler or tape measure with 10ths of an inch on. They are fine for PCBs, but they aren't really Imperial measurements. :) Best thing we ever did was go metric IMHO. It's so much easier - certainly easier than growing extra fingers and toes... Mick Zilog Inside! nascom.info for Nascom & Gemini Preliminary MMBasic docs & my PCB designs |
||||
phil99 Guru Joined: 11/02/2018 Location: AustraliaPosts: 1721 |
" didn't we inherit that from our British Masters? " Only the names. Gallons an tons are under size, even the mile is an inch shorter - if measured in British inches! |
||||
Rickard5 Guru Joined: 31/03/2022 Location: United StatesPosts: 328 |
Thank You Guy's you're all a Wealth of Information I turned the volume on the monitor to max and could hear sound. Thanks Stanleyella |
||||
palcal Guru Joined: 12/10/2011 Location: AustraliaPosts: 1755 |
I keep seeing things like this when buying bolts and screws "It is better to be ignorant and ask a stupid question than to be plain Stupid and not ask at all" |
||||
Rickard5 Guru Joined: 31/03/2022 Location: United StatesPosts: 328 |
SO BACK ON TOPIC : Everything I draw on layer 0 is a cut line ? and is the solder mask auto generated ? Back off Topic, if you're British and Speak the Queen English, Thank an AMERICAN Lathe and mill like the ones that Provided GOODS and Materials in Feet and inches while the Germans were pounding England with French MM. and no I never Use Fractions Rulers and tape Measures are for Psyco SICKOs that find it acceptable to work with Decomposing Tree caucuses. I only work in decimal with Calipers or Micrometers, or a .1"/.01" rule I turned the volume on the monitor to max and could hear sound. Thanks Stanleyella |
||||
Rickard5 Guru Joined: 31/03/2022 Location: United StatesPosts: 328 |
And they wonder why we got a little Snitty 245 years ago? we got tired of getting the short end of the stick :) I turned the volume on the monitor to max and could hear sound. Thanks Stanleyella |
||||
Grogster Admin Group Joined: 31/12/2012 Location: New ZealandPosts: 9030 |
YES - that is something I found also. ALL my own components I design, have 1.8mm pads with 1mm holes for pin-headers. I have found they are a perfect slip-in fit. 0.9mm is a firm fit, and 0.8mm I find to be a hard press-fit. 0.72 default is so tight you have no hope! I use 0.8mm holes with 1.8mm pads for all components including IC pins, resistors, caps, inductors, diodes - everything except pin-headers or other headers, where I use 1mm holes. About the only exception to that, is with the juicy 3A power diodes(1N5404 etc), where the hole is 1.7mm with a 3.5mm pad. Smoke makes things work. When the smoke gets out, it stops! |
||||
Grogster Admin Group Joined: 31/12/2012 Location: New ZealandPosts: 9030 |
Pretty much, yes. 99% of the time, I think it would be safe to say. PCB houses that support V-grooving, use layer zero lines for the V-grooves also, but yeah - everything on layer zero is a cut of some kind. The soldermask is autogenerated by the component IF THE COMPONENT IS DESIGNED TO HAVE THE SOLDERMASK. 99.9% of every component DOES have the pads exempt from the soldermask, otherwise you could not solder to them. But it is up to you. You CAN design components that have pads covered with soldermask, but for all the parts you select from the library, they will autogenerate the mask as you go, yes. Do you have a copy of my Sprint Layout macroes? I can't remember if you have or not. I have designed some 352 different macroes for SL6, and I would be happy to upload a copy here as a ZIP file if you or any other SL6 users would be interested. Smoke makes things work. When the smoke gets out, it stops! |
||||
Tinine Guru Joined: 30/03/2016 Location: United KingdomPosts: 1646 |
Great info guys....keep the tips/tricks coming Confused about layer zero; if I draw a white circle, it doesn't show up as a hole on my print-out. I have to use a pad. What am I missing? Graeme: Not sure if I grabbed a copy of your macros so please re-upload. Craig |
||||
Grogster Admin Group Joined: 31/12/2012 Location: New ZealandPosts: 9030 |
Here are my macros as a ZIP file: MACROS(Graeme's).zip Layer zero is not printed, as normally you don't need it to show up in printouts, as it is a machining layer, not really a layer for showing on printouts. To make it show up when you do prints of your layout, make sure that there is a tick in the "O" checkbox in the print preview window. Click the printer icon on the top taskbar on SL6, then refer to the checkboxes at top-left of the window: Smoke makes things work. When the smoke gets out, it stops! |
||||
Rickard5 Guru Joined: 31/03/2022 Location: United StatesPosts: 328 |
Thanks for the Macros, Grogster the thing I hate about this is, you kids were born in to the Instant Gratification world where you see instant results and can adjust as you go! this Reminds me of the Terror of being a Kid and going on Vacation , and the Holiday snaps come back from the Photomat 2 weeks latter, then Dad comes home all Pissed at the Crappy Photos, so we got to go back to Disney and do it all again! One Year we had to do Christmas 4 times at Aunt Edna's before Uncle Tommy figured out how to snap shots with the instimatic with out red eye I turned the volume on the monitor to max and could hear sound. Thanks Stanleyella |
||||
Tinine Guru Joined: 30/03/2016 Location: United KingdomPosts: 1646 |
I print-off on photo-paper, actual size. Lay the components over the prints to be sure of correct spacing. My board is 400mm X 150mm and so I finally get to use my A3 printer That's been sealed in its box since I received it in May 2019 Craig |
||||
Page 1 of 4 |
Print this page |