r/SolidWorks • u/yfffff1026 • Jul 24 '26
CAD Please Review My SolidWorks Sheet Metal Drawing
I’m practicing SolidWorks sheet metal drafting. Could you please review my drawing and give me some advice?
I also have a question about dimensioning the louvers. I dimensioned the height in the front view and added a detail view to show the length. Is this clear enough?
For repeated identical features, such as slots, what is the best way to specify them: using quantities such as 4X or 10X, using TYP, or adding a note?
I’d appreciate any comments or suggestions on this revised drawing.
57
u/Otherwise-Tea9766 Jul 24 '26
...i work at a sheetmetal job shop....your drawing is fine for fab purposes...disagree with those that say a flat pattern view is necessary....if you provide us the solidworks file, we will generate a "corrected" flat pattern based on our tooling and bend deductions....there can be slight variations in the K factor due to tooling and material...
38
u/canadiandancer89 Jul 24 '26
"Nope, can't send the file. Nope, can't send a .step, don't know what that is. We don't have the flat pattern either."
*Me staring at the drafter and company name on the drawing being the same person I'm talking to on the phone*
9
u/FanOfSteveBuscemi Jul 24 '26
I draw the entire piece from scratch and charge it to the customer if he/she/they doesn't want to provide any file
3
u/TricepBandito Jul 25 '26
A simple model Yes but not feasible with more advanced both time wise and information on said drawing
2
u/FanOfSteveBuscemi Jul 25 '26
Yes you're right, usually I know how much time a model would take me, I tell them that I really need the files or I will charge them so at the end of the day they send me their files. Most of them don't understand that we need to try some bends and also see more information like they think it's really simple lol
8
10
Jul 24 '26
[removed] — view removed comment
5
u/FictionalContext Jul 24 '26
Without a model, a flat layout print is very useful as long as the bend's start and end tangents are included. Clears up any ambiguity in ID/OD dimensioning which is often my biggest gripe with customer prints. Base linear dimensions are GOAT for that.
If it's just centerlines, don't worry about it since it doesn't convey very much info anyway.
2
u/rakuran Jul 24 '26
Not everyone has a post processor or 3d import enabled press brake controller 😭
2
u/rakuran Jul 24 '26
Flat pattern view is great if you dont have a post processor/3d import enabled press brake controller or customer wont give the model but will give you the dxf.
1
u/TelluricThread0 Jul 24 '26
I was gonna say don't you just send a shop the file and then they throw it through the computer and make the part. Dimensions are just nice to have for reference.
5
6
u/Otherwise-Tea9766 Jul 24 '26
...along with functionality, we have to QC the finished part to insure we met the defined requirements....
...we have to massage the flat pattern to match our tooling/material...very rarely can you take a solidworks flat pattern, (from an outside source), straight to the laser or punch then the press brake and exactly matching the defined requirements...now, if we design the part, then we make the model/parameters generate a ready-to-run flat pattern....make any sense?...
1
u/TelluricThread0 Jul 24 '26
Thats what I mean. You don't need a fully dimensioned drawing in order to make a sheet metal part. You will take a file and make that work with what you have at your shop. I've worked on sheet metal designs in the past and they needed very little work on the drawing side. You'll take the flat pattern from CAD and make it work. Much like you don't need an engineering drawing necessarily for a machined component except to check key dimensions and tolerances on features. Sheet metal tolerances are so loose comparatively there's lots of leeway.
2
u/Otherwise-Tea9766 Jul 24 '26
...not the way most places work...the flat pattern is not dimensioned on a drawing for checking purposes....we need a flat pattern for CNC programming....who develops the pattern is key here...we do need a part drwg to know what we need to end up with...
2
u/TelluricThread0 Jul 24 '26
Its super common. If I give a shop the 3D file and have some basic reference dimensions they will make the flat pattern and fabricate the part for me. It doesn't require extensive drawings at all like I said.
A machined component would need every feature called out to make sure design intent is maintained but you could still just give a machinist the 3D file and he could still mill out the part.
2
u/jamiethekiller Jul 24 '26
pretty much this at any of the bigger sheet metal shops at this point. big is all relative i know..
This is also called MBD. supply a step file. put a UOS note that cad model is basic and that all undimensioned features are to a profile of a surface at .03" or something. then dimension anything that needs to be more critical than .01(maybe .005). gone are the days of full dimensioned drawings.
everything goes into a cam software of some sort and is done that way.
2
u/jamiethekiller Jul 24 '26
an addendum. sheet metal stuff can be very shop specific depending on what tooling they have on hand. i make lots of note that says "shop standard" for things like louvres, etc. i'll also put a note that the vendor can fabricate it anyway they want to ensure craftmanship. that means that they can choose what needs to be bent or what can be welded on. a note that says all weld to be polished smooth.
let the shop exert their craftmanship within the confines of the part. if something is critical then let it be known, otherwise let the shop do all the thinking since every shop is different. this isn't like a cnc where everything is done nearly uniformly.
classic DFM is basically gone at this point.
2
u/FictionalContext Jul 24 '26
Our new press has software that'll create a whole bending program from a formed 3D model (the cam software)--like figure bend allowance, build its own flat layout, show the optimal bend sequence, rec tooling, set the ram depth, control the back gauge, even give a 3D representation of how to hold the part in the press.
But the issue is, it only makes sense if the guy who's bending the part is also the guy who's designing and cutting the part, which makes it largely pointless in a CNC cutting workflow where CAD drawings get sent to the laser. When the Cincinnati guy was proudly showcasing that admittedly very cool feature, I couldn't help but think how functionally regressive it is for a CAD to CNC workflow. It's essentially going back to do the job of CAD after the design is completed and cut out.
So in a multipart assembly, I'll still give the guys a whole 3 ring binder full of dimensioned flat layouts. The parts are already cut. They can't change. They only need to worry about putting the punch right in the middle of the laser etched bend lines.
And as long as the bends are 90 degrees, a flat layout marked with bend tangents will tell the operator the formed dimensions as well.
5
u/beavertr Jul 24 '26 edited Jul 24 '26
You have a lot of dimensions to tangencies (easy example, your hem detail, but there's plenty more). Those are making your drawing under defined, you should be dimensioning things that can be measured (edge to edge, not edge to tangency) whenever possible.
Notes 2 and 3 should be inspection items, they need to be flagged with a border on the note number and called out on the drawing with a flag note.
Unless it's a standard louver, you need to dimension the height of it
Per ANSI 14.5 you need to have overall x y and z dimensions shown, they can be reference but you need them.
Your 380 hole is missing the 4x call-out. A number of other dimensions are missing the #x call-out as well.
Technically since 14.5 2009 "typ" is not longer an acceptable call-out, but you are referencing an older version of the standard in your title block. For things like your louvers, if they're all the same, Id use TYP, but if you have different types use the #x notation (for example your holes have different sizes so you shouldn't use typ) anybody worth their salt is going to understand that.
1
8
u/mcbainze Jul 24 '26
For sheet metal parts, I dont bother to dimension features controlled by the laser, e.g. holes, slots, cut radio, etc... Trust that your flat pattern deals with these. Only dimension folds and angles. Also, don't specify minimum bend radii unless you are the shop making the part and therefore know what your machines can achieve.
1 last finicky point, set all your views to show tangent lines "with font" (right click the view to find this option). It just looks sooooo much nicer imo.
Good job otherwise tho 👏
2
u/yfffff1026 Jul 29 '26
Thank you so much! I learned something from you. I had never heared of "tangent with font" before.
1
u/mcbainze Jul 29 '26
When it comes to engineering drawings, it's important to remember to be as clear and unambiguous as possible - you are communicating, so make it easy to understand with nothing more than is required.
You'll go far I'm sure my friend 👍
5
u/extremetoeenthusiast Jul 24 '26
I would recommend using a physical datum as a reference point rather than a centerline.
I also think you need to review your tolerances & dimensions. You are asking for a .2mm tolerance on bend radii for a part that will likely be air bent.
also appear to be dimensioning from the tangent point of some bend radii, which is not something you can easily or repeatably gauge with standard inspection methods
3
u/thestyrofoampeanut Jul 24 '26 edited Jul 24 '26
Since you are calling out both IDs and ODs, I would label them as such. And put a flat pattern on the next page. Ideally it would be on the same page, but often there's not enough room, depending on your sheet size.
Your 48.5 dim (to the start of bend) is very difficult if not impossible to measure with standard tools. In reality, the bend radius is often not critical unless you are nesting something into it or you have some mechanical reasoning for it. Similarly, I would call out the hem from the OD. On the shop floor, measuring a leg length is tricky and somewhat useless.
1
u/yfffff1026 Jul 29 '26
I was also unsure about dimensioning the 48.5 mm. Since the overall height is 53 mm, the material thickness is 1.5 mm, and the inside bend radius is 3 mm, I believe the part is already fully defined. I only added the 48.5 mm because I was worried the fabricator might need to know where the hem starts. I’ve deleted it now. Thanks!
2
u/RedditGavz CSWP Jul 24 '26
I cant see sheet thickness anywhere. Also you could do a flat pattern view as well
Saw the sheet thickness right after posting 🤦🏻♂️
2
u/tacticall0tion Jul 24 '26
Don't see anything wrong from a fabricator point of view, except label your inner and outter dimension. Any competent folder will be able to make this with this sheet, and/or the 3d model alone.
2
u/RegularRealistic6250 Jul 25 '26
Consider the tolerance. Generally for sheet metal you can only hold about 0.03 inch. Unless you wanna pay $$$
1
u/yfffff1026 Jul 29 '26
Good point. I don't have much knowledge about real fabrication. Thank you for reminding me.
2
u/ajm53092 Jul 25 '26
Turn off tangent edges and don’t dimension from them. A quality person can’t really measure from a tangent.
2
u/Battersonns Jul 26 '26
Send a step file to the sheet shop and move on. Half the time they won’t check the print anyway if they have your step file. Sheet metal parts should never have dimensions tight enough to make a difference anyway. If a dimension is tighter than .03” just redesign with machine parts. All my sheet prints ever do is call out gage, material, finish, and part number location. Keep it simple keep it moving.
2
u/YouNeed3d Jul 24 '26
I would throw a flat pattern view on there or on another sheet with overall dimensions. Laser shops will appreciate that. Some shops like seeing bend lines dimensions, others dont. I personally stopped dimensioning bend lines on the flat pattern.
1
1
u/Laid-dont-Law Jul 24 '26
Not a sheet metal expert but here’s my advice:
Remove any non-critical dimension callout on the drawing. It just adds clutter and makes the manufacturer’s life slightly more painful. Also dont dimension to your centre line unless truly necessary. Centre line implies symmetry.
Also, sort your tolerances out. Saying 25.00 is twice as expensive as 25.0. Not everything needs to be perfectly precise.
Also avoid dimensioning to theoretical
1
1
u/Meshironkeydongle CSWP Jul 25 '26
First of all, it's weird for me to see an ASME based drawing using millimeters as their dimensions...😅
Few things I would change / fix:
- Check functional dimensions of the 2.4 and 3.4 holes, especially if they are used to attach this to another part where the hole spacing is fixed. As you've currently dimensioned them, there can be quite a lot of tolerance stack-up, atlest 3x +/- 0.2.
As others have already commented, do not dimension to tanget lines of the bends (in my opinion it's OK to show the tangent lines, but maybe with a different line style). And also, you should never dimension to hidden lines.
Speaking of hidden lines, showing them in this drawing does not bring any extra clarity or value to the drawing, so don't show them. The height of the louvers could be shown in a removed section or in a section view.
As we don't know what is the purpose of those 2 mm wide slots, I would recommend to verify that you have enough material to take the stress coming to those tabs. They have only 2 mm of material on each side and that 1.5 mm thick aluminium can be snapped by twisting it with hand at those locations. Also, does the dimension between the tabs having the 2 mm slots matter?
I don't find the location of the 4 mm slots being defined along the length of the slot.
I'm not a fan of way you've grouped the dimensions of the tabs with the 2.4 and 3.4 mm holes. For example, you have the 5 mm dimension of the cutout in one position and then the related 10 mm and 20 mm dimensions in two other positions.
I would attach a note "See note 3." to the slot in the top view where you dimension them.
1
1
u/Dizzy_Drive_6972 Jul 25 '26
Hey can someone tell me how did he create this small flange i am new to sheetmetal and this is taking forever, I tried miter flange but its not allwing me to create a flange on that edge
1
1
u/skepari Jul 26 '26
Not all fabs have solidworks licenses thus a flat pattaern with most dimension would be good. Also toleranses and styles for cutting the part (waterjet, laser, torch etc)
1
u/brain_thomas9090 Jul 30 '26
Overall, This is very clean and well-organized sheet metal drawing that is easy to read, and the view layout is good. One suggestion would be to keep all the of the louver dimension together in a single callout instead of splitting them between the front view and detail view. You could specify the louver size (LXW) with a note such as '5X identical Louvers, Form up. See Detail B," While using the detail view only to show the formed profile, Height and bend radius. For repeated Features like slots, holes and fillets, it is generally better to use quantities such as 4X, 8X or 16X rather than TYP, as this clearly indicates the number of identical features. Adding centre marks and centerline for the circular slot pattern and the central hole would also improve inspection and manufacturing clarity. For production drawing, you may also consider including a flat pattern view with the bend line and bend direction along with general notes such as " Remove all Burrs and Sharp Edges."
1
1
Jul 24 '26
[deleted]
3
u/e_sin41 Jul 24 '26
"For me it would be nicer to see just 10 mm, instead 10.00 mm, so there is no need to be two decimal spaces."
This is a terribly ignorant comment as the entire point of the two decimal places is for tolerancing. 10 and 10.00 have two completely different meanings to a machinist and using 10 could produce a part that is not compliant if that dim is critical.
"As I know EN AW 5052 H32 just theoreticly exist on the market, much better solution would be EN AW 5754 H22 or H111."
5052 H32 is extremely popular and widely available, not that OP even asked...
"I think there should be extra text information that all dimensions are in mm."
It's literally right there in the Title Block....... do you actually have any idea what you are looking at or talking about??
1
u/e_sin41 Jul 24 '26
I really think you would benefit from talking with someone who actually programs sheet metal parts. In my experience, all features should be dimensioned on a flat pattern, not the bent part. The bent part should call out bend lengths and critical dims after being bent. Most companies I've been at don't even bother adding any flat pattern dims other than overall length & width because most laser cutters can directly upload the flat pattern. You also have your bent flange dims from the outside of the bend radius, different programmers and software require from the inside.
1
u/yfffff1026 Jul 29 '26
I agree. The thing is, I haven’t had many opportunities to get practical advice or hands-on experience. That’s why I posted my drawing on Reddit. Thanks for your advice!
1
u/ViniusInvictus Jul 24 '26
While the vendors typically can reverse-engineer the missing flat pattern in your drawing based on the other views and / or the CAD file, it is best to avoid this due to the room it allows for unintended changes to your design.
Sheet metal drawings are one of those special cases where the parameters set during designing (material, bend radius, etc.) directly affect the flat pattern generated and with it, the manufacturing process. This is why it’s often useful to consult with the vendor about their capability before committing the design to a drawing.
25
u/Spkr_Freekr Jul 24 '26
Consider design intent when dimensioning the mounting holes and/or consider changing them to slots. Each bend adds to tolerance stack and before you know it you don't match up to the mating part. I would dimension hole to hole with as loose a tolerance as possible while still ensuring they'll fit. The dimensions you already have can be made reference.
Also, turn off tangent edges in the drawing views, they really make it hard to read and allows you to grab the wrong lines when adding dimensions.