Detached drawing has been a tool available in SolidWorks for many years. It allows drawings to be opened and used without the need to immediately load the associated model or assembly. The idea is that you can load a drawing much faster when you don't intend to make any changes to it.
My question is, do you use Detached Drawings? If so, how? If now, why not?
SolidworksDrawings And Detailing
I don't. My drawings seem to load fast enough.
YES - (sorry for yelling) - I like things right at the source and that is where I would see it be the most valuable, off - on * on - off
I have some time while waiting for my models /drawings to open and close while I am experimenting with the detached drawings. I will attempt to learn how to do that.
There is also an option to load the model when opening a detached drawing already. (See snip below) Not sure why the speedpak is there as my testing showed if there is a speedpak in an assembly the option to save as a detached drawing is not available.
Nice find, Grant. Would be even nicer if the Load model checkbox would be made available for all drawings. So we would no longer have this confusion between "drawings" and "detached drawings".
I tried a different drawing that has been taking a co-worker quite a bit of time to open. I saved it as detached and then closed SW. Upon opening the detached drawing it took 10 seconds. I was able to navigate the drawing and add dimensions and balloons. I then closed and opened the attached drawing and it took 5-1/2 minutes to open. That is a big savings.
Exactly what I am seeing too. Amazing that this tool isn't more popular or discussed. Great solution to our large assembly drawing issues. A few more tweaks by SW and it will be a perfect solution.
I just tested opening a detached drawing (of a large assembly, without the model open) and adding a large number of dimensions. Very good response from SW with minimal delay adding the next dimension. (Works as expected) I then did a "Load Model" on that view and repeated adding the same dimensions again and the response was the same. I currently believe when the load model command is used it only updates the views with any new lines and has no further negative impact on the detached drawing. I am not yet convinced Unload model would do anything more then what the detached drawing already does. If we can choose to open any drawing as a detached drawing that would be the next major step.
Great feedback, !
We should spend a morning together, Jim. I am pretty sure we can find many other opportunities for time savings!
The concern I have is a repeat of what happened in the past, where not properly rebuilt or updated drawings were released for production and incorrect components were made. It's just like everything else, to have good stuff coming out of the pipeline good stuff needs to be put in, also needs to be in a controlled environment. I can't wait till all the enhancements go through on this, thinking is an awesome start.
For now this can be solved by implementing a simple procedure, like the one I suggested earlier.
For now, use it only for detailing. To be safe, add a big watermark on the drawing: Detached - Do Not Print or Release!
Also, I believe that a detached drawing would give you a warning when it is out of date.
Apparently I should have checked before I asked for something as it already exists. I will report how well it works after I test.
The biggest problem I see, as I sit here waiting for a drawing to open, is that you have to open and save the drawing before you can detach it.
Yes, but you do that only once. Also, if you follow the workflow we listed here, on drawing creation, the pain is even less.
That is probably why Grant is looking to automate this process. So he can do the conversion unattended.
See circled (sort of..) in read above.
Won't that be a problem? Detached drawings are NOT broken links....right? Not technically. Right?
Let's test is first.
#Task worked exactly as I hoped. Now I just need to check their new PDM plugin and convert a bunch of drawings to detached over night. If everything works as planned the person working on these drawings tomorrow is going to be extremely happy.
Once we have even more trust in #task and detached drawings we won't need to use any extra prefix or suffix.
Amazing. Looks like brainstorming can uncover hidden gems.
Thanks, Grant!
ER 1-1386215092 created to detach, reattach and re-detach on the fly. Included request to be able to update only active view to request.
I have about 50 drawings of large assemblies set to save as "Original name_Detached" overnight using #Task. I'm looking forward to the results in the morning. I will post here with how it goes.
Thanks, Jim. Please post here the SPR number once you get it.
I actually want to post this before someone makes a fuss about it.
Detached drawings work by the views being "high Quality", if you have been around long enough you may have tried to save a drawing as either a dwg or pdf and ended up with blank views. This is caused by the view not being "High Quality" but "Draft Quality". Now why might a view not be converted to "High Quality" you ask?
Almost 99% of the time it is because of geometry errors.
Solidworks does provide a tool to check for these errors, it is located in the "Evaluate" toolbar called "Check"
Another useful tip for anyone troubleshooting a large drawing, when attempting to convert a view to "High Quality" the processing is down in the background but if you switch over to the tree and expand the sheet node you will see a very small hourglass icon that will disappear once the conversion is finished.
I did not have an actual screen shot so I just sketched it in.
#Task worked well for me last night and I have about 50 new drawings that I will do some spot checks on. Jason I did run into the issue of not having High Quality set on some of the views and they came in blank. Thanks for getting your post up about draft quality before I was frustrated this morning. Also interesting to note the file size, on one of the drawings with draft quality views, is 555mb. It still opened as fast as other detached drawings but all views were blank. I will have to see if there is a way to switch views to HQ with #Task.
I will post here if I discover anything else interesting or frustrating with the new detached drawings.
Great feedback, Grant. How does it feel to do research?
I love R&D and don't get to do it as much as I like. Currently I am starting to get behind of my own deliverables though.
I am finding a couple things with detached drawings:
1. File sizes seem to get large when a 3D shaded view is used. Need to investigate if it is all shaded views or just 3D.
2. Something has caused a number of drawings to believe they are out of date when opening. I thought it was some blocks in our drawings that are not used but I deleted them, saved and reopened and still have it. There are a couple dangling dimensions in the views as well so I am currently loading the model and will attempt to reattach/delete to see if that is the issue. If that does not solve the issue I might need to get some other ideas from people here.
3. The 555mb file that had draft views set in the original still did not work when set to HQ before saving as detached. The newest version is now 640mb and took 45-60min to save. The open time is still amazingly quick even with a file size that large. Maybe has seen this before?
1. A view using a Shaded display style is by default a draft quality view.
2. If you find out that it takes too much of your time to investigate this issue, ask for help from your VAR.
3. Does the new version contain HQ views?
It is expected for a detached drawing to be larger than a normal one, considering that it has to store all the information needed for printing, zooming and detailing.
Thanks for the reminder about shaded views being draft quality by default. I did switch all views on this drawing to HQ before saving them as detached.
Below is a different drawing with a shaded view in draft quality saved as a detached drawing and it works.
I agree about the increased file size for detached drawings. Typically I have seen about a 2x increase but the 640mb file is now 19x large then the original, just seemed a bit extreme.
Unfortunately we don't all have VARs named Alin.
Actually, for this type of problem solving, you do.
Alin ??? Alin who ??
Yes, you can save in DQ, but remember, you will save all triangles! That what makes the drawing huge.
Matthew,
We use Detached Drawings but I am not quite sure as to why. File size is larger. If it's sent to a vendor or customer it seems to still send model info. What is the intent from Solidworks for Detached Drawings?
Hi Grant,
We have the following macro to convert all views to High Quality, but if there are model issues (Geometry Errors) the views will fail to convert to High quality.
Solidworks and PDM will always have a warning that the drawing is out of date, we have this notification turned off in PDM.
Disclaimer: Needs a loop for each sheet!
Also use at own risk et cetera
-----------------------------------------------------------------------------------------------------------------------
Option Explicit
Public Enum swDisplayMode_e
swWIREFRAME = 0
swHIDDEN_GREYED = 1
swHIDDEN = 2
swSHADED = 3
swFACETED_WIREFRAME = 4
swFACETED_HIDDEN_GREYED = 5
swFACETED_HIDDEN = 6
End Enum
Sub main()
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swDraw As SldWorks.DrawingDoc
Dim swSheet As SldWorks.Sheet
Dim swView As SldWorks.View
Dim bRet As Boolean
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set swDraw = swModel
Set swSheet = swDraw.GetCurrentSheet
Set swView = swDraw.GetFirstView
Debug.Print "File = " & swModel.GetPathName
Debug.Print " " & swSheet.GetName
While Not swView Is Nothing
Debug.Print " " & swView.Name & " [" & swView.GetDisplayMode2 & "]"
If swSheet.GetName <> swView.Name Then
bRet = swView.SetDisplayMode3(False, swView.GetDisplayMode2, False, True): Debug.Assert bRet
End If
Set swView = swView.GetNextView
Wend
End Sub
-------------------------------------------------------------------------------------------------------------------------------------------
You will also see that the file size will increase, a normal drawing when saved converts all views to draft quality to save on file size.
So it does make sense that a drawing saved as detached is saving the drawing with all views as High Quality.
There is also a setting that may help overlapping or coincident geometry appear correctly, in document settings\Image Quality\Precisely Render overlapping geometry(higher quality, but slower).
2016 SOLIDWORKS Help - Detached Drawings
Well put Alin!
Grant Mattis wrote:
Thanks for the reminder about shaded views being draft quality by default. I did switch all views on this drawing to HQ before saving them as detached.
Below is a different drawing with a shaded view in draft quality saved as a detached drawing and it works.
I agree about the increased file size for detached drawings. Typically I have seen about a 2x increase but the 640mb file is now 19x large then the original, just seemed a bit extreme.
What are your settings here:
and here:
These are my current setting in a detached drawing. The circled item is set to HQ on my computer and DQ on another test computer. It is the one that is set to DQ that is currently showing up with blank views. I have not tested that same file on my computer yet. Both computers are checked to save tessellated data.
I might try a few things over the weekend and let the computer do the work. Hopefully I have something more to report by Monday. I am getting pushed to focus on deliverables but this is really important to keep moving forward for anyone that deals with large assemblies. I'm sure detached drawings have lots of other purposes too just not what I need them for.
The weekend was just too nice here to do any indoor work but I managed to do some testing this morning.
I have a number of drawings with a single 3D shaded view and 1 drawing with 8 shaded views. The drawings with a single shaded view are all set to HQ and appear exactly the same when opening the detached drawing. The 8 shaded view drawing was saved exactly the same way as the others, with HQ views, but it opens as hidden lines removed with no shading. I would like to do more testing to see when this flip happens but I am out of time.
I did also find it interesting that if I had the model open before I opened the 8 shaded view drawing that the drawing opened with the views shaded.
I will try to follow up with this thread occasionally and let everyone know how the detached drawings are proceeding in a real production environment. Hopefully some or all of the SPR's that we have discussed in this thread get implemented soon.
Does anyone use detached drawings for something other then large assembly drawings?
Emailing drawings to contractors who do detailing (adding all the dimensions, non-parametric notes and more), without giving them the models.
That is a good idea if using an outside contactor for detailing drawings provided there will be no updates to the model that the contractor will need to detail. I could batch create the detached drawings with #TASK and send them in the morning. File sizes might be a bit large but should still be way less then sending the model. I might start using that method for those situations.
I will be running detached drawings through a real test shortly. We have a 60 page set of submittal drawings that need to have some small revisions for our customer. Some of these drawings take over 20min to open right now so I really look forward to having them open in 30 seconds or less.
For many years I have used www. mailbigfile .com to send all large files, easy and quick..
Ran into a slight issue/inconsistent performance of detached drawings. We have noticed that some notes linked to part properties do not update correctly when using detached drawings. I did not expect notes to be able to pull part properties correctly without the model loaded.
First picture is showing we copied a note and pasted it to the same part. Second picture is showing that after doing a load model the part properties are updated. This is great and exactly what I expected detached drawings would do. The issues start happening in picture 3 & 4 so please read below.
We did the same thing with the note below in the 3rd picture of this post but when we pasted the note or tried to create a new one it was like the lines/part are not actually there. In the 4th picture you can see that the note did not update. I know the note in the example is pulling very limited information from the part so not the best example but this might be a deal breaker for us using detached drawings. It wouldn't be a big deal if this was only one part on a detached drawing but it is about half of the objects in a view sometimes they are sections and sometimes detail views. There just does not seem to be any logic to these notes working or not other then if the lines can be selected it seems to work.
I was impressed though when I did a load model this same part is now selectable and a pasted note updates correctly. Also worth mentioning when a detached drawing is loaded all new notes linked to part properties seem to work appropriately. The detached drawing with a loaded model does seem to operate slightly slower but still much faster then a regular drawing. It would be a shame if we need to load the model every time we open a drawing just to add notes like this. I really want to delay loading the model until exactly when we need to do it.
I am very open to other thoughts or suggestions. I did search the knowledge base and was not able to find any solutions or current SPR's that discuss this issue.
I am trying to understand why sometimes drawings could be saved as detached in seconds or minutes, and other times it takes a whole day. I am talking about comparable size drawings, with comparable number and types of drawing views, depicting comparable complex assemblies.
What is your experience with the time it takes to save drawings as detached?
We typically use #TASK to save out our detached drawings. I keep the timeout set to 45min and haven't noticed an issue with the saving time. Sorry I couldn't be of more help. I'm interested in this issue though in case we face it at some point in the future.
TL:DR Sorry if this is somewhere above...
Isn't a PDF a form of Detached Drawing?
Uhhhh....no.....You can't edit things in a PDF or add dimensions and stuff.
Well, I suppose you COULD do those things....but you would be using whatever PDF editing software you had....and it would be slow....and it would suck.....and it wouldn't update the original drawing.
Damn, really? I'm going to try using one here today that is pretty complex.
Steve C
Really. SOLIDWORKS is close to solving the Large Assembly Performance problem, but not for large drawings.
The Detached Drawing tool is one of the most effective for bridging the gap between the Quick View mode and the Resolved mode.
We just need to work together (users, VARs and SW) to further develop and clean such tools.
The Drawings Environment needs more love from all of us.
So, since I'm using Smarteam as our PDM system, I'm a little scared to try this but I'm going to give a 4 sheeter a try and check it in. I'm wondering what happens since the file extension is the same the regular drawings vs detached drawings.
Steve C
It behaves as a regular drawing if you load the model.
This is a decision you can take when you open the drawing (check the box Load Model), or anytime once the drawing is opened.
What happens when a drawing has views refering different models? If I select a view and click Load Model, only the model for that view should be loaded.
That at would be very helpful, allowing some views to stay detached, while enabling the use of one of the models to update other views, or generate new views.
COOL!
Just tried doing a detached drawing (4 sheets) that has a large assembly used for the views in our Smarteam PDM environment and it worked as designed. Great job SW... The drawing opens in a few minutes vs. a lot of minutes (I also did some large assembly maintenance like finding and fixing all mating errors and rebuild errors and creating one or two "SpeedPak" sub-assemblies).
Now I get to go find these large drawings and their assemblies and detach them.
Steve C
Excellent Steve, I didn't know Smarteam still existed! I used it at 2 places that I worked, back in the early part of this century...how time flies! Glad it worked out well for you.
Yep, we use it and it's in 6 places around the world.
THX
Steve C
Cool. I liked it, a bit cumbersome, but we had facilities in France, China, Brazil, & Australia, besides the USA. I wasn't an admin, just a user.
Did you use detached drawings in Smarteam? That was what I hadn't tried before and we have some large footprint drawings that took a long time to open because of the attached assy. I've cut the open time down to several minutes.
Steve C
No, I'm not sure if it was invented back then! I started with SolidWorks 98 Plus back in 99!
Great Steve. Those must be some really big models ours are big but typically open in less then 30 seconds. Make sure you don't have the model/assembly open when you open the detached drawing or it automatically does a "load model" and is significantly slower to open.
Yes, the idea behind detached drawings is that you don'y need to open the drawing.
Good tip...
Steve C
Great news, Steve! Also, keep in mind, as wrote, you can perform batch detaching using #TASK.
I don't really understand the logic behind this thread. SW please provide the business rules used to develop the feature in the first place. What was it originally designed to accomplish?
Personally, I don't know why a person would spend $5,000 on CAD tool to load a detached drawing in the first place. If you are just viewing the drawing then use a blasted viewer tool or view a pdf. They are either free or very low cost.
If this tool was "designed" to reduce the amount of time to load a drawing of a large assy then why not just a function to the drawing view to "Freeze" the view from updating or the drawing sheet itself. In the NX world we can load a large assy 3 million+ component assy and update drawings or I can load the drawing sheet and "Extract Edges" from the view. Then when the assembly is loaded with no components I can still see what the drawing "last" looked like when the components were loaded.
As I mentioned it would be good to understand the original purpose for the function was.
the biggest reason for me to want to start using them is because SW doesn't load drawing fills like Unigraphics used to and many times all someone needs to do is open the drawing and change/add a note. In my case, all we're doing is updating a note to show the people in the field how our gasoline dispensers are installed at the site. I don't need the model opened so detached drawings make that faster.
Steve C
Quoted from the Help files;
Essentially that's the basic benefits of it in a nutshell Kelvin.
Dave.
I for one don't think it was a feature that was actual designed. I suspect that someone figured out that if a certain bit of code wasn't nudged then the result would be a detached drawing.
If you then consider that there are some, a few but some nonetheless, instances that something like that could be handy for some and that it could be touted as a 'new feature', well..... it's easy to see how it became a 'thing'.
For those that once in awhile have a need for it, great. But as this thread clearly shows (only 10 pages of posts in 5 years), the need for it is not often nor very frequent.
I'm hoping that SW figures out how to do all assemblies and drawings so that they open many times faster. I know they've made improvements from release to release but I'm now wanting leaps of times. I'm ok with us (the users) figuring out how to make our assemblies and drawings open faster by doing certain things, but I'm sure the geniuses at SW are close to solving this.
Steve C
I'm with you on that one Steve!
9 of those 10 pages were written in the past 2 months.
As more people become aware of this feature, as any other, more people may come to appreciate it!
For printing or viewing we have instant access to the drawings already. Is called opening in Quickview mode.
We also have settings that provide full control to the user on when to update drawing views.
"Detached drawing" is a misnomer, in my opinion. It just adds another layer of control, allowing the user to decide when to load the model and when not to load it.
Is is great not only for opening drawings fast for detailing purposes, but also for operational purposes on older hardware. You will find that detailing the most complex drawing works super-fast on the crappiest workstation.
In my opinion, SOLIDWORKS confused users when named this functionality "Detached Drawings". It scared all the people who did not take the time to try it, it scared all managers and IT technicians and gave unwarranted ammunition to people who know a different CAD system well and try to compare it with SOLIDWORKS functionality that they do not fully understand.
Yes, quick view is good for just that, a quick view, but you can't do anything with it other than look at it. You can't even add text (at least in 2015) which was mentioned above!
Alin I was one of those people. Why would I want to detach a drawing? Can I reattach it again? No way I am going to try that feature. I was pushed to try it to solve our issues and I had the model open when I did so it wasn't actually any faster. We discovered through testing that Detached drawings do an automatic "load model" if the model is open. Simple solution and now Detached drawings are part of our normal workflow on large assembly drawings. With a few further tweaks that were discussed in this thread it could be an even better tool. Maybe rename it at the same time so users are not scared.
Grant
You also had a great enhancement idea. The ability to unload the model, after all drawing views get updated. That way, you ensure you have the latest update for your drawing, but the detailing can be performed really fast.
That is what a detached drawing is good for. Detailing with the speed of light.
Excellent idea Alin!
Matt, would you agree that this statement is incomplete? When we do not need to change drawings, we use QuickView mode. Detached mode is for quick detailing and revision jobs.
Detached drawings do not open correctly in many cases. I recently opened a case# with my VAR about this. We had a drawing with 30 sheets, most sheets had detailed parts and in the notes the material was linked to the model. Every time i opened the drawing some views on some sheets would not show correctly and the notes would not show the material (that was linked to the model). a sharp tech figured out by doing a save as, it showed file type "detached drawing". As far as we know, there is NO other way to figure out if you have a detached drawing now or not in the latest versions of SolidWorks. I saved it as a separate regular solidworks drawing file, deleted the detached drawing and problem solved.
Now i would like to search and find all the detached drawings, and save them as regular drawings, or at least make a list so i know how many we have. Back in the day, sw had a separate icon for them so they were easy to spot. not anymore. The VAR told me there is an SPR out asking to bring back the "blue icon" for detached drawings but as usual my hopes aren't too high.
so what happens is people that don't know the views and notes aren't fully rebuilt when they open it, they make a PDF and send it out. then the PDF isn't matching the original solidworks drawing, and other problem; drafters go through and re-do the notes on 30 sheets, then find out it does the same thing next time they open it and they waste a 1/2 day trying to figure out what's going on with the drawing.
one other note, if you're using them just so you can send drawings to people and they can open them without all the parts and assemblies, or having to install edwg, there's a way to do this without making detached dwgs. just use sw, and select quick view mode when you open the drawing, it will show any sw drawing without needing the parts and assemblies
What happens if you simply load the model, instead of performing a save?
the problem in this case was that we did not know it was detached, so if you mean by loading the model, that you right click the sheet and select load model, then yes, that would work. However, if you don't know it's detached, you don't think to do that.
so now that i know, i could open it, then right click hit load, THEN make my PDF.
however, other people that open it do not know this, so they don't think to do that. there's no more indication that dwg is detached anymore within solidworks or the windows icons.
we only have a few, old legacy drawings that are this way and i have no way of finding them. saving them as a regular drawing solves the issue.
everyone in my user group i've talked to stopped using detached drawings years ago simply because it doens't load the model(s). we don't care if it loads a little quicker if it doesn't display certain things correctly, then you have to right click and hit load model, may as well just be a regular drawing file and then it loads correctly every time. i'm surprised they even allow saving as detached drawings anymore.
Here's an idea: tinker with the drawing file format such that it can be opened view-only in Acrobat.
and.... forget about e-Drawngs???
, I agree! Knowledge is power.
Advanced tools like SpeedPak or Detached Drawings should never be used by untrained users! Never, ever!!!
In any company, the use of such tools have to be governed by written procedures to be used by fully trained users. The benefits are worth the investment in time for training.
If you read earlier in this thread, has already listed the limitations of the Detached Drawings, including the problem with custom properties values when the model is not loaded.
I agree with the icon. It should be made very clear in all environments. Right now it actually is visible in some environments.
By the way, you could load the model directly from the opening dialog. Just check the "Load Model" checkbox.
Hi Alin,
we are kind of going in circles here. I would consider myself an advanced users, as well as the individual at my company that couldn't get the notes to update correctly. The VAR i sent it to spent a number of hours on it and showed it to other techs there, who also couldn't figure it out. finally he stumbled upon the File, Save as, and happened to see the detached drawing in the filetype menu, otherwise we would all be trying to figure this one out three days later. It's not so easy when you do not know it's a detached drawing.
Seems easy to fix looking back, but at the time not so much
I've been using 3D PDF lately instead of eDrawings. It's gaining fans amongst my peers and clients. No special viewer required and no EXEs!
You would be surprised how few people, (including VAR AEs and SOLIDWORKS Technicians), are aware of the Detached Drawings functionality. I started studying them only after I needed to solve a critical problem for a customer.
This thread provides a wealth of information about best practices for using Detached Drawings safely, along with a lot of Enhancements Requests for SOLIDWORKS. I really hope reads this.
Take a look at all the posts from in this thread. Maybe we should compile all of the best practices, pros and cons in one post. We will do that soon.
Examples of places where the Detached Icon is shown in SW 2017. I agree, that the difference is barely noticeable. , we need a new, bolder icon to indicate the Detached state.
1. Feature Tree
2. Windows Explorer, if the thumbnails are off
detached drawings sounded good till you wanted to make a change......
think that it was something that the other cad users wanted when they moved over to SolidWorks like the layers.....
Being a SolidWorks user with out a the pdm system makes you a top notch file manager....always thinking about what this change is going to do to all the places it is used......
the Idea behind the detached drawing was for when you or someone went to make a change to something or it just got all fouled up due to no fault other than that of having a really bad day at your file management..........
To do a detached drawing it is much easier to just do a save as pdf....print to pdf...and then you can share the drawing with just about anyone,......
This is precisely why I am concerned about using many of the "advanced" techniques. While they do save time and can make life easier for the one in the know, the next guy to come along may not be thinking about that technique when he attempts to work with the model. Everyone here has been using SW for at least 5 years but the company isn't big on spending money on training. Documenting things in the model helps some but there are still things people would have a hard time figuring out.
Hi Allen, we are aware that within the file there are ways to tell if the drawing is detached.
but if you have 2000+ drawings, and you have to open them all to find out, that isn't going to happen. as far as the icon you show, i have tried every setting, thumbnails, no thumbnails, big, small, list, thumbnail preview on and off within sw. my icons look like this for regular (on the left) and detached (on the right). if you can tell me how to get the old icon for detached to show up in sw 2016, or sw2017 drawings, within windows, you would make a lot of people very happy. please look at the images. I cannot see a difference.
Detached Drawings sound great and is a Great Tool in a company that has different departments or if you need to work on very Large Assemblies. Totally get what is saying and highlighting the current issues, someday it'll be standard practice. Here I am the only person using SW and I don't work with large assemblies, so there won't be a need in saving any drawing as a detached drawing... Cheers
Once they are compiled we need to give the information to so he can get it linked in his fantastic Excel search tool.
Then either you or John or maybe need to pick up the torch from Matt Lombard. We need a new tips and tricks Bible.
That's for sure!
lol - Me.... What are you drinking? - no Matt Lombard needs to carry the torch... He lit it, at least be a Co-Author...
Do you use PDM? If you do, please vote on:
SPR 625667: The icon of Detached Drawing data in Enterprise PDM should be same as Windows Explore.
You might be right. He might have rights on the SOLIDWORKS Bible name.
Due to his new job's constraints, Matt can no longer write about SW.
Mark,
Here are the icons that I get in windows. These icons only show up like this outside of PDM. If I were to view them in PDM then the icons are exactly the same. SW2016, PDM 2016, Windows 7.
SPR 625667 is to fix the icons in PDM. I posted it earlier in this thread somewhere as well. Please vote it up and let SW corp know how much time you lost due to the issue and also that your VAR had problems finding the issue as well.
Grant
Check this : Catching up from a 4 Year Sabbatical
Sorry Alin apparently I was writing my response while you posted. Mine does have the nice picture of the different icons though.
Cool. IMHO, you can write a new book focused only on the what's new in SW since 2013.
It looks like @Matt_Lombard has been busy lately!
well, at least you can see them i do have pdm, however, the first thing i did, and my var was to see if the icons work in windows, and in pdm. neither me nor my var could get them to show in either
let's dig a little further if possible, maybe we can figure this out, do you have Windows 7 service pack 1 & SW 2017
(that's what i'm running)
Mark I have Win7sp1, SW2015sp3, SW2016sp5 & PDM 2016 installed. Maybe it is a difference in our SW versions.
I have the same OS and SW 2017 SP 4.0 EV.
Update: after working with my var neither they nor I can get "detached icons" to show in windows, which stinks. apparently some people can, but we can't figure out how. tried every Windows and SW settings we could think of, various versions, different computers, etc... And, SW has an SPR out on this from some other users trying to do the same as me, find all my detached drawings without having to open them. For those who do not know, in the "old days" SW used to have a detached dwg icon, and it showed up fine on everyones PC, but the file extension was likely different back then, now its the same as regular SW dwg's (.slddrw) so windows cannot distinguish.
My goal is to find all my detached dwg's, and save them as regular drawings. opening every drawing to find them is not an option.
i'm on the SPR notification list, so If SW can fix or figure out this SPR I will certainly come back here and update the thread to let people know what the fix is.
Thank You for listing your OS / SW versions, much appreciated
Interesting. If you want to post a detached drawing here I can see what my computer does with it. Even if it is a simple cube saved as a detached drawing it would be interesting to see if my computer recognizes it.
sure, thanks for checking
Very interesting. My computer does not show a difference in icons for your two drawings. I assume the drawing labeled detached is actually detached as it is in 2017 and I can't open it here. I have included a screen snip below and also included a detached drawing I created on my computer showing the different icon for reference.
Maybe it has something to do with not having saved and opened the drawings myself or that they were not created on my computer.
I think SPR #625667 should get this issue fixed so everyone please vote for it if you are able.
Grant, thanks for doing that. The issue must have started with SW2017 then, because the one labeled detached IS a detached dwg. when i open it, it shows the detached icon on the top left, and when i click 'file, save as' it shows detached as the file type.
This is just one more reason not to use detached drawings. The interesting thing is that i thought maybe they had a different file extension in older versions of SW, but yours shows ".slddrw"
learn something new everyday!
we'll just have to wait to see if SW can fix this in the SPR they have on it.
I sure wish I knew more about this month and month ago....I have some very large assemblies... in the order of 25k components...and working in the drawings took way too long, would take between 10-16min just to open a drawing file. I think I've reached the limits of SW...I'd be lucky to get a sheet a day. I came across some threads in here about detached drawings and seemed promising.
Just saved as a detached and took secs to open now...I'm hopeful I can zip along now and not lose my mind anymore...
SW is very poor at large assemblies...grant it most people are only dealing with at most 50-100 components...
I know what you mean, at my former place of employ, we had huge assemblies with 10K parts and 200 different design table driven configurations-one radically different from the other-some times opening or saving would take 3-4 hours, you just found other stuff to do while waiting...I don't miss it LOL
Good news! Grant's Large Drawings presentation has been accepted for delivery at SWW2018!
Thanks for sharing and congrats - sure it will be great
, Grant and I just tested this assumption on a model with topological errors. The detached drawing works fine and the drawings are high quality.
Do you have an example where the behaviour is different?
Mark,
When I opened up your detached drawing file, it shows the detached drawing icon.....
Bob
Hello,
Haven't used it.
I'm only in an SW drawing long enough to create it or modify it, then it's saved as a PDF for production.
Like our PDF files, when we recieve files from a customer, the PDF is the authoritative document.
If SW files are also provided, their use is generally secondary: generate a flat pattern DXF, checking an omitted dimension, etc.
Since most of these tasks involve the part or assembly file only, the drawing is only opened to verify the SW is at the PDF revision.
When a customer sends a SW drawing without its part or assembly, I open the drawing resolved as Quick view to be conversent (and keep things rolling) while the customer gets the omitted files to me.
Cheers,
Kevin
Hi Jason,
Two things. One I recommend to check the "stringent" option in the evaluate property window. Two, and that is what puzzles me the most, why is SW not flagging the issue. I have come across this problem many times especially with large assemblies but also with individual parts. I took me a long time to figure this trick out. It's a real bugger to troubleshoot especially with large assemblies & drawings. If you don't know about it you are sure to waste lots of hours.
I think SW should provide some sort of feed back if the view does not convert to high quality i.e. "Problem with Draft Mode - Do you want to check assembly for errors - Yes/No" That will save heaps of time. I am glad that with 2018 we can now identify the components that have errors....Previously you had to custom-macro around to deal with this.
Elmar
Hi Matthew,
Detached drawing benefits sound great. I would most certainly like the advantages, only and only if SW can make the drawings reliable.
No errors! Saving 20 min of drawing time versus, building something based on a drawing with errors is no saving, it's a loss.
Another is dimensions loosing the reference points. No point for me adding stuff only to find out I have to do it again because it lost its attachment for one reason or the other. And I don't mean model changes. More magic software behavior.
Creating views and then adding dimensions is a very simplified way of thinking. I have to add linked notes, balloons, welding symbols and yes of course dimensions just to name a few. But I have to spread all of them out to make the drawing readable. So working in detached mode to add some dimensions is of little help. Revision work maybe, but only if the parametric update is reliably populated to the drawing.
Maybe another approach would be better. Often I work in a specific view or two. Not all at once. If I could toggle the views itself detachable.
If SW could release computing power since I don't have to recalculate all views then maybe that would make things faster. I don't know, SW is the code expert here. And when I save & close the drawing it would update all views to make sure I have a current status.
Alternate views are anther issue. They are essential a drawing view pasted over another so they use up computer power. And they make dimensioning harder as the slow down draft's men. Often time I can't even pick entities because the two interfere with each other (work around Hide alternate view - dimension - then unhide alternate view again)
But key is reliability. A drawing is the last piece of document that leaves engineering and the number one document used in production.
If that is incorrect...well do that once or god behold a few times and a "...but I used detached drawings...yada yada" is gonna be your last words on the way through the door.
Elmar
Hi Elmar,
Have you tried Detached drawings? I agree they are not perfect but if you know the limitations and are able to deal with them you can save a lot of time with no extra errors.
You have some other great suggestions and ideas for detaching specific views to free up resources. I can see that working really well for those resource hogging sections views or configurations.
I have been very busy this year but time is a little more free now. Hopefully I can join back into the conversations here a little more.
Grant
I have a drawing with several views (front-top-side-isometric) including a section view. Because it slows the drawing so much I've made it a detached drawing making it easier to annotated and putting some dimensions on it.
I'm now regretting it. Because the model has been updated but because of detached view it doesn't update the drawing. I've spend the last 2 hours trying different things, up to and including saving the detached drawing as a 'normal' drawing and nothing seems to do the trick.
All it results in is the program being unresponsive.
Have you tried just loading the model?
Alin,
Yep, if contacted my VAR. We looked at it for the 45 minutes. Trying everything he could think of but to no avail, including safe modes.
I though that it used to be that if you loaded the model first that the detached drawing would update automatically but either I was wrong or that doesn't apply any more.
Any thing we tried to get the views updated involved loading the model, even if the model was pre-loaded and in all cases it just made the program unresponsive (hanging).
In the end I remade the drawing, that took me an hour as well but at least it updates again with the model.
Hi Peter,
I have used Detached drawings a fair amount and I have not seen this issue. We are currently on SW2016 so maybe this is an issue in a newer or older version.
I have used the "load model" during detached drawing opening successfully, "load model" while already in a detached drawing and doing a save as back to a regular drawing. I have not had any of these methods fail yet.
When you say SW hung opening a detached drawing with the model pre-loaded did you give it enough time to open. I have detached drawings that open in 30 second that take 20-30min to open the normal version. Just want to confirm it is actually hung.
Can you let us know what version of SW you are using so everyone can watch out for this issue.
Thanks,
Grant
Peter, was a SR filed for you, or did your recreation of the drawing close the issue for the VAR?
Grant,
I'm using 2018SP3. The longest I waited was 25 minutes and all I got was an utterly blank screen during that time.
Matthew,
No I didn't file an SR. And yes me recreating the drawing was closure for me and the VAR.
I need that drawing now and it could just as well be that it's a fluke, a one off, in which case me spending time and effort on uploading files and getting an SR filed is for nought because nobody is going to look at it unless it turns out to be something that others experience as well.
IF I should happen it again with another drawing then I'll file an SR.
Hi Matthew Lorono
Saving a drawing file as a detached drawing so we have some level of editing power without having to load the linked part or assembly file.
we can use it by following steps:
1. Open the model and drawing together .
2. While saving the drawing save as detached drawing in the menu list .
3. After that close all the part related documents.
and then open the detached drawing and make the changes as required in an easy way..
I hope this ans. your question...
Hi Solidworker!
Cool to hear about the use of macro to assist the Detached Drawing. But, I just want to know that for what purpose the macro is used to assist the detached drawing.
Cheers!
Co-Solidworker.