So heres what im trying to do. Below I have an enclosure that I have created out of sheet metal members. What i need to do now is make flat pattern drawings
I am using SW2014 SP5.
One method is to RMC on the Cut List folder in the feature tree and select Save Bodies.
This will save out each body as a separate file.
However, the saved bodies will NOT be sheet metal. You will need to perform a convert to sheet metal on each one and collect all bends.
If you have hole wizard holes you will need to re-establish these if you want them to be recognized as such. I create a sketch and convert entities of all the hole edges and then fill. I then use the hole fill sketch to define the hole locations of a new hole wizard feature. This maintains the parametric location. Yes, a real pain of a work-around. Perhaps this is no longer necessary in newer versions of the software.
Once converted to sheet metal, you will have an individual sheet metal part that will flatten.
To help clarify, we save our bodies out as described more to jive with our workflow than anything else.
Here, each body would be a separate part number. And each part number gets a drawing. And burying different part numbers inside of a part is not handled by Workgroup PDM - at least as far as extracting BOM information.
J. Mather's approach is valid. But it doesn't fit our company workflow and file management.
Daen,,, Sounds like you would like to have an assembly, of what you are showing, with individual part files. If so, how about deleting the base feature of each part you want to exclude from your part file (you can keep any necessary sketch geom) and then saving that to a part number of your choosing. Open your multibody part file anew and do it again for another part until you have all the parts saved. Now you have functioning parts of each with all the info you put in. You then can begin a new assembly and simply insert the new parts. Don't drag them in. Just select the part you want then green check. The parts will come in fixed and in their correct positions. So you may want to unfix then mate.
In your assembly file.
Here is a screenshot of a file I tested this on. Not as complex as yours but think it should work. This started out as a single multibody part file.
Edit:.. I probably should add that if end up with a bunch of dangling sketch geometry (on edge stuff), and it is too much of a chore to fix that, use delete bodies and live with that in your new part files.
When I follow your OP, where do the files get saved?
Never mind I found them.
You will need to perform a convert to sheet metal on each one and collect all bends. If you have hole wizard holes you will need to re-establish these if you want them to be recognized as such.
You will need to perform a convert to sheet metal on each one and collect all bends.
If you have hole wizard holes you will need to re-establish these if you want them to be recognized as such.
I just stumbled upon this and was just wondering if this is still the only way to do derived sheet metal parts?Trying this usually led to an abundance of errors, especially when the faces changed after changing the geometry of a part a bit. Sometimes we could not fix those parts & so we went back to making configurations for the parts (slower but way more stable results).
You should also be able to create a Flat Pattern for each body and then select each one individually for drawing creation without writing out the individual part files.
On occasion - I have had trouble with that though and often have other reasons to have each body in it's own file.
Here is how I handle a multi-body sheet metal part:
1. I see you have 20 bodies, so in the Default configuration, do 20 separate Delete Body commands.
2. Now create 20 additional configurations. (Part01 to Part20)
3. Use Configure Features so that each Partxx configuration has its associated Delete body command suppressed.
4. Go back and suppress all those delete body commands in Default configuration. (This sequence saves on mouse clicks!)
4. Now create a drawing for each Partxx configuration. I have Sheet 1 as the bent shape.
5. Add a second sheet and insert the body, but select Flat Pattern. This will force SolidWorks to add the Flat Pattern derived configuration to the part file.
6. Repeat 4 & 5 for the other 19 parts.
In effect you have created 1 assembly and 20 part files in a single multi-body part file. I assign configuration-specific part numbers ,etc.
Now any changes in Default will be reflected in the Partxx configurations / drawings / flat patterns.
I'd be using #TASK for this.
If you just want the DXF's use the "Export Flat Patterns" task to export your multi body flat patterns straight to DXF.
Or if you want SolidWorks drawings from them, use the "Sheet Metal Drawings" task. It will create a single drawing file with the flat patterns on it. You could then use the "Drawing Splitter" task to separate into individual drawings if needed.
So following Daen's OP I have run into this twice on two different parts that are both round. Some advice would be great.
Yes, this has been a behavior of SW for.... every maybe. The typical work around for this is to add a very small straight section to your large curve to act as the base flange. Small means like 0.03". Enough that the software can use it but insignificant to your part. Yes, it does change your part dimension. But you can usually size the flat flange to be smaller than your tolerance.
I don't do Sheet Metal everyday like I did a few years ago..
I did try multi part sheet metal and I guess I'm too ignorant or too old school, or to set in the Sketch Part ways, but really isn't it much simpler just making individual parts? For individual custom properties, ease of parametric changes...........
My process is definitely NOT for everyone and it does have it's pains. Here are a few screen shots to help clarify a little more...
Here is a frame weldment with sheet metal bodies. The frame will be built in-house. But the sheet metal blanks will be laser / water jetted by a vendor.
The sheet metal bodies are saved out to separate files.
Here is the saved sheet metal body. It was converted to sheet metal. Next holes were filled. This is done for two reasons: SW looses Hole Wizard info when the bodies are saved and if you want to benefit from the parametric hole call out tool in drawings this is a necessary step. And sometimes holes need to be added AFTER the structure is welded.
At the end of this feature tree, there is another SAVE BODIES. This creates the BLANK part that will be sourced from the outside vendor. Remember, these steps are much more about process than the best or slickest way to perform this in SW. Since different vendors are blanking and bending (whether internal or external vendors) the blank needs to be separated from the bent part as far as part number and tracking. If we were to send this to a sheet metal shop that creates their own blanks and performs there own bends, then the whole "separate blank" process would not be performed because that is "their" internal process instead of ours. In that case we just order the part number of the bent form.
The corresponding drawing with a note calling out the use of an existing blank...
And here is the blank... "lather, rinse, repeat" regarding the convert to sheet metal and in some cases filling holes.
Is all this a ROYAL Pain in the Dark Side! Absolutely. But it is process driven. Managing this type of thing through configurations, which most of you do, would be much less initial work. The down side is that method buries P/N 456 inside of part file 123. We are still using Workgroup PDM and it does not have the ability to pull configuration specific BOM data - such as the P/N 456 noted above - for reports or importing into our ERP. You also loose the nice functionality to open a drawing by Right Mouse Clicking an open part/assembly and selecting Open Drawing because the drawing for the sheet metal is a different file name than the drawing for the multi-body part. The use of a single drawing to contain all the drawings for all the bodies creates the same issue of burying drawing for P/N 456 inside drawing for P/N 123. I would then also have to send the entire drawing to the sheet metal vendor with an explanation to ignore this and that. "I" also would have to do that task. I couldn't use our ERP system and just order it because the folks that make all that happen are not in the engineering department. They would have ZERO sense that to find all the information for 456, just look in 123. They would have no sense of the "caveats" to explain to the vendor.
In a nut shell, more work up front, WAY less mistake later on. Pay me now or pay me more later....
As I said above, this process is NOT for everyone. But here it is for your review and maybe it will give you something to consider.
Hey Dean, I came across your answer to the sheet metal/weldment issue while trying to pave my own way to come up with something that works well with Workgroup PDM, 3rd party CAM software, ERP and outsourcing, and now it seems that for the most part I was following in your footsteps. In saying that have you experienced any issues using your process? Do you think it's faster or slower? Anything you've done to speed it up getting your parts from a multibody part to going through your system such as macros? Do you use any methods of batch generation of body properties to name your files? I assume you use the save bodies function to batch save all your bodies into new parts using the name you gave the body property, so have you ever had to deal with a duplicate part? Since Solidworks won't let you name the cut-list item it looks like it's hell bent on making you save identical parts under different body names (since the number is applied at the body name). It makes sense that you want to do this in case one body gets a modification and now the duplicate body is two individual bodies. I've been working on something that'll speed up one of our processes for a really long time and this is the first I've heard of someone more or less proving out the ideas I had zeroed in on. I apologize if that was a lot of questions but it got me a little excited to see this.
I had forgotten about this post. You have several good questions.
Have I experienced any issues? Few issues as far as functionally broken. A number of annoyances and inefficiencies. If model updates result in adding or removing bodies, updating the Save Bodies feature can be flaky. As noted previously it involves a lot of steps. To propagate changes usually requires all of the files to be open and ctrl-Q rebuilds to be "walked through" each file in order of the saved bodies lineage. Other "hobbyist" users of SW in the company have a hard time grasping the workflow - not to replicate it, but just to follow it.
Faster or Slower? For me it is subjectively faster. But that comes from performing the process regularly; completing all the tasks and putting it to rest in my mind; not having to be interrupted later to explain, create, generate any sort of files or documents for others. It is also faster for me because it is a consistent process - I don't have to spend hours chasing down rabbit holes trying to figure out what someone else has done with a model.
Any process improvements? This process would be a prime candidate for a macro. Unfortunately that sort of thing in this company is not encouraged - I was hired to Engineer and CAD, not program; we have too-busy programmers with zero SW exposure that are much better skilled at ignoring such a project.
Batch Generation? As the CAD design starts to firm up I create Part Numbers and Descriptions in our as-of-yet unlinked spreadsheet of P/Ns. This, at least, allows me to rename the cut list items to match all at once. Duplicate bodies get an addition to the P/N name to differentiate - usually a position (LH, RH, Top, Back, etc). The cut list properties are copy/paste from the P/N spreadsheet. Otherwise, this part of the process is still very manual. Something a macro would manage nicely. You can see this in the first image (cut list) in my original post.
I do use Save Bodies. I may have more than one Save Bodies feature. Sometimes I will break it up on body type (sheet metal vs. weldment profiles). Sometimes SW absolutely will NOT let me do all the bodies in one feature due to modeling particulars. Sometimes model revision updates result in Save Bodies feature updates and the software breaks so I relent and just add another. The body name is the Part Number. If there are duplicate bodies with the positional add-on to the name then I have to edit the Save Bodies proposed body name back to just the P/N before saving. With duplicate parts, I just save one of them out.
I am not sure I understand your meaning when you point out that SW won't let you name the bodies. It certainly won't allow duplicate bodies to have the same name - hence my positional add-on mentioned above.
I would be happy to expand on any of your questions or clarify my answers. My process could certainly use some improvements. I have been using it long enough that it is my standard workflow, is familiar, and because of that is efficient (for me), and provides a robust end result.
Unfortunately I do not have any update information - I am still limited to using SW2014 SP5. I have read through the "What's New" documents for every release of the software since and I do not recall any specific discussion of enhancements to converting sheet metal.
To mitigate the errors that changes cause, I tend to push creation of the whole "Save Bodies" work flow until the parent CAD design is pretty well established. That may not be feasible for everyone.
Retrieving data ...