HopeRF RFM95W LoRa Module

https://www.hoperf.com/modules/lora/RFM95.html

Fritzing Part:
RFM95W_LoRa_Module_v1-2.fzpz (15.7 KB)

SVG Files:
RFM95W_breadboard_v1-2 RFM95W_breadboard_v1-2
RFM95W_pcb_v1-2 RFM95W_pcb_v1-2
RFM95W_schematic_v1 RFM95W_schematic_v1

That’s a pretty good part, just needs a bit of changes.
The traces anchor to the centre of the pad, and if a trace takes a sudden turn it will over lap the next pad. To fix it you set the terminal point to the W for the left ones and right E for the right ones.


You can code it in XML, but you will have to look that up.
Also the right pads are cut off on the PCB, so you need to select all in INK and Edit/resize to selection. Same for the BB
In XML the g66 needs to be renamed silkscreen, or bring the buried group SS to the same level as copper1 and delete the unused above groups.

I have updated the part and SVGs.
But i’m not sure what the problem with cut off section in the PCB and Breadboard view created.


Anmerkung 2020-06-13 101844
I noticed that the dimensions of the part were different after the import with Fritzing.

I did start the parts in Inkscape with mm as the unit for the page width+height. The original measurement of the part are 16x16mm. That is why i chose that. But Inkscape seems to convert units different from what i expected.
Anmerkung 2020-06-13 101845
(screenshot of the page settings of the BB SVG)

When i turned the units to “in” it did convert the numbers. But they were not equal to the ones of the Viewbox settings. I played a little bit the viewbox settings and managed to make them equal to inch value of the page width+height. But afterwards i needed center everything on the page. The page frame is now a little bit bigger than necessary but nothing gets cut off.

I have updated the part and the SVGs again because the distance between the solder pads was not exact anymore.
It seems to be the best to set the display units and the units of the page width and height to the same unit and to adjust the scale factor of the view box.
Anmerkung 2020-06-13 121809
If one switches the width and height unit to inches then the view box values have the same decimal places. (But i still do not understood the context completely.)
Anmerkung 2020-06-13 122026

I think it’s the transforms.

Select group in INK XML Editor, ie, silkscreen, ungroup to base. Then without clicking on anything else - everything in that group is still selected -, regroup and rename, ie, silkscreen. That gets rid of transforms and it should go into FZ at the right scale.

Hmm. Is the FZ parts not alright? (It looks right to in Fritzing and Inkscape.)

Sorry I tend to not read the whole response because it’s too much work :slightly_smiling_face: . I thought you had to fudge the “Resize the part to selection” size in INK, ie, it had to be bigger, so that it would import into FZ the right size.

@Faizan2020: Unfortunately, I have no time in the next days. (Lets keep the discussion here: STOCKO connector design)

But this is paid work and I will pay you for this work if would invest your time.

Here is an improved version of this part and the changes made:

breadboard

import pdf for layout!

Here I imported the board image from the pdf file then scaled it to match the board and added/moved components to make breadboard closer to the actual board. Renumber connector15/16 to 14/15 to remain in sequence (likely a parts editor bug!)

pcb

remove the connector terminals, they aren’t needed in pcb. Change pin to pad (SMD pads as opposed to through hole.)

remove text. Text can be added by the user to the sketch but can’t be removed if it is in the part without changing the part, so typically the pcb svg shouldn’t include text! Change pin15/16 to pin14/15 to remain in sequence. Added a dot to silkscreen to mark connector0

schematic

replaced with the template file and reduced size somewhat.

fzp file renumbered pins 14/15 and changed pcb pin to pad for smd pads. Added a bus for the 3 ground pins.

edit Mar 2023

Replace original part (where pcb pads are too wide) with a corrected part.

RFM95W_LoRa_Module_v1-2-improved-smd-fixed.fzpz (19.9 KB)

Peter

1 Like

@ntm
@vanepp
I’m unable to change which PCB layer this part resides on a single layer PCB.

bottom seems to be the only option on a single layer PCB.

Yes, because there is only one copper layer on a single sided pcb, so it will only go on the bottom (as it is SMD) in order to connect to the copper. If it was on the top it would not connect to anything. Through hole parts will change from top to bottom on single sided.

edit:

although I see when I look at breadboard that it is actually a dual part (SMD and through hole) and thus should have a through hole version which will do what you want. I’ll make one in a bit.

edit1:

OK here is a through hole part. Note that the holes are set to 0.038in (suitable for .1in headers) which are likely too large for the 2mm headers this looks to use. You should also print out the pcb footprint at 1:1 scale and check that the holes align with a real part (it is less important in the SMD version and I am assuming the OP got the positioning correct …)

edit2: I replaced the part with one with the holes set to 0.031in which shows as the recommended value for a 2mm male header.

RFM95W_LoRa_Module_v1-2-improved-tht.fzpz (20.1 KB)

Peter

1 Like

Thanks for the part. I’ve used PCBWays online tool for viewing the Gerber files and final PCB as they would make it, and this part seems to have quite large pads with not much spacing, larger than the footprint on the actual part, when seen in Frizting the pads are sized more in line with the actual part. I’m not sure how I adjust this. Any idea on what needs to be tweaked just to shrink these pads down.

Pads and spacing that will be created on the PCB
image

Which part are you using? The RFM95W_LoRa_Module_v1-2-improved.fzpz part two posts above has smaller SMD pads. If they are still too large they can be easily made smaller.

Peter

Thanks for your reply, I’m using the version 1.2 improved. In Frizting PCB view the part appears okay, but the solder area is much larger when previewing the Gerber files. I can’t see how the part can be edited to correct the issue, I gave it a go, but can’t see where the solder paste area for the pads is set.

While I’m far from an expert on pcb fab, it looks fine to me. I think you are looking at the solder mask layer (not the paste layer.) This is the gerber displayed in gerbv this is copper1 and the solder paste layer

the paste layer covers only the pad as I think it should (I assume but don’t know for sure because I don’t usually do SMD) that the paste layer is used to make the stencil for solder paste. The solder mask layer is larger (as it is blocking the solder from spreading beyond the pad.) and forms the typically green solder mask on the board. Neither is directly modifiable in Fritzing, they are automatically generated by the gerber processing AFAIK.

I believe this is showing the edges of the solder mask (the entire area other than the copper will be filled with mask I think.) It looks to me like your viewer is displaying the solder mask layer as the paste layer for some reason (but checking with the board house would likely be a good bet!)

Peter

Thanks for looking into it.

I’m just using PCBWays Online Gerber Viewer - PCB Prototype the Easy Way - PCBWay Gerber viewer just to check the design, but the same larger pads are noticeable if exporting as PDFs from Fritzing and looking at the etch mask so not an issue with the Gerber files or how PCBWay are viewing them.

Attached are two parts, one an ESP 32 Wroom and the HopeRF as viewed using PCBWays Gerber viewer. I’ve selected to view just the copper, and the pads are pretty large for the HopeRF, much larger than depicted on the Fritzing PCB designer and much bigger than they need to be compared to the part itself. The ESP32 part to compare, the pads are much the same as seen in the Fritzing designer. When I select the solder mask on PCBWays viewer, the area depicted for the ESP32 pads are a bit larger, as of course the solder mask is a bit bigger than the copper area, but on the HopeRF part, the pads have so little space between them the solder mask just covers the entire row of pads, so no solder mask between the connections.

So it seems to match your design you screenshot above, but the pads are much too big in my opinion.

I have a Lora Node with an RF95 on it, and the pads are nothing like as large (https://www.tindie.com/products/iotmcu/lora-radio-node-v10/) . The pads just need to come out onto the copper etching layer the same size as they shown in the designer. I couldn’t see anything editing the part in Fritzing parts editor, what software should I use to tweak it?

Expecting something more like this

image

The current pad size appears reasonable to me. It is set in the pcb svg file via Inkscape (or another svg editor.) Here I imported an image from the data sheet and rescaled it to match the footprint (which has the correct 2mm pitch.) The pads look reasonable in both width and height.

This is what the pads should show up like in the gerber output which should be correct according to the data sheet. I don’t have one of these boards so this could be wrong but it appears to match the datasheet. From the picture above the real board looks to match the datasheet and should thus be right. The other image you are using looks to be a module such as an ESP32 with a finer pad pitch (this is an ESP32 WROVER module)

which is the wrong pitch for the RF95W module

You look to be comparing apples to oranges.

edit:

I forgot to add the best suggestion: Print the pcb footprint (such as from the pdf export) out at 1:1 scale on overhead transparency paper and compare that footprint with the real part. If the two match the footprint is correct (and the transparency lets you see that the footprint indeed matches!)

Peter

The ESP32 example was just to show that other parts behaved as expected.

With regards to the part in the datasheet, the datasheet isn’t showing a recommended footprint, so some interpretation is needed. Your image and the copper pads are lined up incorrectly though, the copper pads are shown in between the constellations, this would short out every connection

The copper pads should be underneath each connection point. For example:
image

However the copper pads are sized okay, and this is how they show in the Fritzing design view, so in Fritzing I see.

image

So that looks bang on, decent gap between connections due to correctly sized pads.

However when it is exported for fabrication, it shows as below, much bigger pads with less space in between, this will likely short out when soldered as there would be too much solder paste for the given area of the pad.

image

Other parts in Fritzing export to Gerber just fine and there is no change in pad sizing between the part as shown in Fritzing PCB designer and what would be ordered with the manufacturer.

Have you ordered a PCB using this part, and did it work out okay?

Anyway I will just create the footprint part manually using pads and the ruler to get them spaced spot on, just thought it was a shame to have gone to all the effort of creating a part which appeared to be wrong at the point of exporting and ordering a PCB.

Thanks for your time.

Yes I know, and they do, I purposely offset the pads to the pdf to show the pad is the right size. The second image is offset in y to demonstrate the length of the pads.

No, as noted I don’t have one (and in fact I just fixed this part up, I didn’t make it.) That said it still looks correct to me using gerbv and I expect that it should if I ordered boards. If it is indeed wrong I’m all for fixing the part, but at present I don’t see an error. Perhaps I will try and use the viewer you are using and see what it says and go from there. It looks to me like the viewer is displaying the solder mask layer as the copper layer which would be incorrect. I would suggest printing out the footprint on transparency and compare that to a real part, but you are of course free to do what ever you want.

edit

I used the referenced site and it still looks to me like their error. They look to be rendering all the layers with no differentiation (gerbv used different colors for different layers.) I can’t see any way on their web site to suppress layer display other than not providing the layers.

here is their output with only copper1 provided. This is what the copper layer will look like I expect.

capture

this is their output with all layers loaded (the layers are listed on the left side of the image but you can’t change them)

It indeed appears broken because they are rendering the solder mask layer over top of the copper layer, but I believe under the extra layers the correct copper layer exists (as shown in the image above with only copper1 layer supplied.

This is the diagram from the pdf, gerbv copper1 and your site’s copper1 only output rescaled in Inkscape. To me that pads look correct and are the correct size. If I ordered this board from elcrow (who I usually use) I would expect it will work. I can’t say about PCBWay because I have never used them, but this appears to be a web display issue not a gerber error in the part. The copper1 display from PCBWay appears to be correct and I expect that is what the copper should look like on the board.

Peter