I'm working on a custom design for a friend for a dirt-bike disc brake rotor. I did the basics, circles, extrude and after that extruded cuts for holes, some round, some odd shaped, inserted some text, ext.cut, circular pattern on most of the items and ended up with a 13Meg file. I'm saving for a new PC and handling such a big part file for this two year old is a really hard task. I thought that with many surfaces I got, there might be a way to reduce the size of the file without losing the important and valuable data. That exists for music and image files, so I thought there might be a trick I could use if available. The part alone is not a problem, but where will it end if the disc which is one of the 300+ components in a bike alone takes up 13Megs... Will I end up with a 10G assembly file for the whole bike ?
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Reducing part file size - possible? 3
- Thread starter steinmini
- Start date
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1
- #2
steinmini,
To learn what is driving your file size you should go to Tools -> Feature Statistics. This will rank the most computationally intensive features first. If your text is turned into a feature it very well might be ranked first.
A simple trick that may help is to suppress everything and save the file with the instructions to unsuppress all after opening. For temporary file size reduction (it may be enough to e-mail) you can do a File -> Save As (Copy). This new file should be much smaller until it is opened in SWX. (This is pretty much what EcoSqueeze and another program did.)
There are also internet file postings where you post the file and send an e-mail to the recipient with instructions on downloading. If neither of you have access to FTP then this might be the best bet.
- - -Updraft
To learn what is driving your file size you should go to Tools -> Feature Statistics. This will rank the most computationally intensive features first. If your text is turned into a feature it very well might be ranked first.
A simple trick that may help is to suppress everything and save the file with the instructions to unsuppress all after opening. For temporary file size reduction (it may be enough to e-mail) you can do a File -> Save As (Copy). This new file should be much smaller until it is opened in SWX. (This is pretty much what EcoSqueeze and another program did.)
There are also internet file postings where you post the file and send an e-mail to the recipient with instructions on downloading. If neither of you have access to FTP then this might be the best bet.
- - -Updraft
rstupplebeen
Mechanical
I agree with Updraft that the text is probably the culprit. 13MB is really not that large though for a part. You may be able to reduce the rebuild times and file size by turning some of your odd shaped hole geometry into fitsplines. I hope this helps.
Rob Stupplebeen
Rob Stupplebeen
- Thread starter
- #4
The last curved cutaway pattern appears to be the most consuming. 43% of the resources... Text follows with 15%. Didn't get any smarter with this, similar patterns within the same file are much less resource consuming (ok, will not ask how come or why)
Anyway, it's not a problem for me to store or send the file, file sharing services are widespread, but I obviously did not ask properly, so the answer can't be what I anted to find out (the answer I got was useful, anyway
)
I'll try to rephrase my question:
Would a different approach in modeling (using different techniques to get the same final shape/design) reduce the size of the file? Storing is not a problem, rather handling and manipulating it later on. Or should I just shut up and experiment?![[ponder]](/data/assets/smilies/ponder.gif "[ponder] [ponder]")
Anyway, it's not a problem for me to store or send the file, file sharing services are widespread, but I obviously did not ask properly, so the answer can't be what I anted to find out (the answer I got was useful, anyway
)I'll try to rephrase my question:
Would a different approach in modeling (using different techniques to get the same final shape/design) reduce the size of the file? Storing is not a problem, rather handling and manipulating it later on. Or should I just shut up and experiment?
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1
- #5
CorBlimeyLimey
Mechanical
Experimenting is always good ... providing you have made backups first.
- Thread starter
- #6
Here's what I've got for the second time:
Feature Statistics:
metaldanske rotor 205mm 5/4/2010 7:33:18 PM
Features 27, Solids 6, Surfaces 0
Total rebuild time in seconds: 101.87
Time % Time(s) Feature Order
43.05 43.85 CirPattern17
15.36 15.65 CirPattern4
13.17 13.42 CirPattern15
11.90 12.12 CirPattern16
4.32 4.40 Cut-Extrude14
3.48 3.54 CirPattern10
2.16 2.20 Cut-Extrude16
2.01 2.04 Cut-Extrude15
1.91 1.95 CirPattern6
1.18 1.20 CirPattern5
0.92 0.94 Cut-Extrude9
0.11 0.11 CirPattern3
0.11 0.11 Cut-Extrude8
0.08 0.08 Cut-Extrude11
0.08 0.08 Cut-Extrude13
0.05 0.05 Sketch3
0.03 0.03 Sketch13
0.02 0.02 Sketch11
0.02 0.02 Sketch2
0.02 0.02 Boss-Extrude1
0.02 0.02 Sketch1
0.01 0.01 Sketch6
0.01 0.01 CirPattern1
0.01 0.01 Sketch12
0.00 0.00 Cut-Extrude1
0.00 0.00 Sketch9
0.00 0.00 Sketch15
The CirPattern 17 (the most consuming) is visible as light blue curved line on the inner edge of the braking surface. that's what confuses me...
Anyway, I'll try to get the same or very similar design with fitsplines...
Thanks to both answers. I'm attaching the image to be clear what I'm talking about.
Feature Statistics:
metaldanske rotor 205mm 5/4/2010 7:33:18 PM
Features 27, Solids 6, Surfaces 0
Total rebuild time in seconds: 101.87
Time % Time(s) Feature Order
43.05 43.85 CirPattern17
15.36 15.65 CirPattern4
13.17 13.42 CirPattern15
11.90 12.12 CirPattern16
4.32 4.40 Cut-Extrude14
3.48 3.54 CirPattern10
2.16 2.20 Cut-Extrude16
2.01 2.04 Cut-Extrude15
1.91 1.95 CirPattern6
1.18 1.20 CirPattern5
0.92 0.94 Cut-Extrude9
0.11 0.11 CirPattern3
0.11 0.11 Cut-Extrude8
0.08 0.08 Cut-Extrude11
0.08 0.08 Cut-Extrude13
0.05 0.05 Sketch3
0.03 0.03 Sketch13
0.02 0.02 Sketch11
0.02 0.02 Sketch2
0.02 0.02 Boss-Extrude1
0.02 0.02 Sketch1
0.01 0.01 Sketch6
0.01 0.01 CirPattern1
0.01 0.01 Sketch12
0.00 0.00 Cut-Extrude1
0.00 0.00 Sketch9
0.00 0.00 Sketch15
The CirPattern 17 (the most consuming) is visible as light blue curved line on the inner edge of the braking surface. that's what confuses me...
Anyway, I'll try to get the same or very similar design with fitsplines...
Thanks to both answers. I'm attaching the image to be clear what I'm talking about.
Experience and going through the SWX tutorials and help (and this forum) are the best teachers in the long run.
Looking at an image of your part without the tree only tells so much, but here is some advice:
1. Name your features as you create them. Nobody goes back and names them later. This is one of the best habits you can develop. It makes your file easier to work with now and when you revisit it in a year or pass it along to someone else.
2. Look in this forum in the Whitepapers, FAQS and Search to find best practices. You'll find links to blogs and websites of individuals and companies that have a tremendous value.
3. Learn multiple ways of doing things in SWX. (I used to never use a sketch pattern because they drew a huge vacuum. In 2010 they made big improvements so I am revisiting sketch patterns.) For instance, a) learn the difference in making a single hole wizard hole and then patterning it versus making all the holes in the same hole wizard feature, b) putting fillets/radii in a sketch vs. creating them as features following the main features, c) creating sheet metal from a bending perspective vs. making the part and turning it into s/m at the end.
Judging from the image it is evident you have some decent skills with SWX, but you did ask for suggestions.
By the way, why does your part have more than one solid body? From the single view we have there doesn't appear to be a reason for this. Perhaps this is contributing to your issue.
- - -Updraft
Looking at an image of your part without the tree only tells so much, but here is some advice:
1. Name your features as you create them. Nobody goes back and names them later. This is one of the best habits you can develop. It makes your file easier to work with now and when you revisit it in a year or pass it along to someone else.
2. Look in this forum in the Whitepapers, FAQS and Search to find best practices. You'll find links to blogs and websites of individuals and companies that have a tremendous value.
3. Learn multiple ways of doing things in SWX. (I used to never use a sketch pattern because they drew a huge vacuum. In 2010 they made big improvements so I am revisiting sketch patterns.) For instance, a) learn the difference in making a single hole wizard hole and then patterning it versus making all the holes in the same hole wizard feature, b) putting fillets/radii in a sketch vs. creating them as features following the main features, c) creating sheet metal from a bending perspective vs. making the part and turning it into s/m at the end.
Judging from the image it is evident you have some decent skills with SWX, but you did ask for suggestions.
By the way, why does your part have more than one solid body? From the single view we have there doesn't appear to be a reason for this. Perhaps this is contributing to your issue.
- - -Updraft
- Thread starter
- #8
Updraft,
for #1: When making something "useful" like parts for my trikes from which I have to derive technical drawings for the machinist, subcontractors etc, I always give name to all the created features. This is just a project for fun and learning and appears as a useful way to find out something new.
#2: This forum is huge and so far I've spent hours and hours and feel I'm still at the first crumble, OTOH, before I started making my first part in SW, bought two books and got through all tutorial videos found over the Internet, plus got two dvd's with video tutorials
#3: this is exactly what I was asking about. The experience so far shows there are always at least two ways to get to the desired result.
My knowledge about the SW and ways it can be used and my skills are really modest. Most of the years I'm designing recumbents I spent making drawings with Corel and a friend recommended SW as a way to go. He was right. Once I saw what can be done and with what ease, I could only ask myself a question why did I wait so long. However, there's a lot to learn in the years to come. To be honest, two month ago, the best I could do in SW was to draw a square or a circle and to add dimensions to it. I hope my learning curve will continue the same way as it did so far and that in a near future, I'll be able to post more answers than questions. For now, I'll try to do the same thing in a different way and keep checking the features to see where do these solid bodies pop up.
Excuse me for my English, it's not my mother tongue, but I do try to make myself understandable.
... and a star for Updraft for being more than just helpful
for #1: When making something "useful" like parts for my trikes from which I have to derive technical drawings for the machinist, subcontractors etc, I always give name to all the created features. This is just a project for fun and learning and appears as a useful way to find out something new.
#2: This forum is huge and so far I've spent hours and hours and feel I'm still at the first crumble, OTOH, before I started making my first part in SW, bought two books and got through all tutorial videos found over the Internet, plus got two dvd's with video tutorials
#3: this is exactly what I was asking about. The experience so far shows there are always at least two ways to get to the desired result.
My knowledge about the SW and ways it can be used and my skills are really modest. Most of the years I'm designing recumbents I spent making drawings with Corel and a friend recommended SW as a way to go. He was right. Once I saw what can be done and with what ease, I could only ask myself a question why did I wait so long. However, there's a lot to learn in the years to come. To be honest, two month ago, the best I could do in SW was to draw a square or a circle and to add dimensions to it. I hope my learning curve will continue the same way as it did so far and that in a near future, I'll be able to post more answers than questions. For now, I'll try to do the same thing in a different way and keep checking the features to see where do these solid bodies pop up.
Excuse me for my English, it's not my mother tongue, but I do try to make myself understandable.
... and a star for Updraft for being more than just helpful
My suggestion is to create two configurations. One config is detailed and would be used for your drawings. The other config would have all of the intensive stuff suppressed. Use this config in your assembly. That way you can point to your part in the assembly and not have to deal with the slow down due to complexity.
-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist
-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist
- Thread starter
- #10
I was already thinking about that possibility. I had a problem with building up the wheel from the hub I designed with spokes nested properly into the holes both on hub and the rim. At the end, I decided it's easier to "cheat" for the complete model where the hub #2 will take it's place and that one differs only in minor details but is good enough for presentation, user manuals etc., and of course, it has cylindrical holes so concentric mating will be possible. Hub #1 remains for technical drawings and for what it was designed. So, precise and detailed drawings and modeling when and where required, and "false" models where only appearance matters. Sometimes it's less work doing some things twice
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1
- #11
Don't use a different model, use a different configuration. Do a SolidWorks help search for configurations. Configurations allow you to have "alternate" versions of the same part contained within the same part file. This functionality is one of their primary uses.
-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist
-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist
Can you attach the part file here - I suspect it can be modeled under 2meg.
Since it is so large drag the bar below the last feature to the top of the feature tree to roll up all features. Save the file in a rolled up state. Right click on the file name and select Send to Compressed (zipped) Folder. Attach the resulting *.zip file here.
Since it is so large drag the bar below the last feature to the top of the feature tree to roll up all features. Save the file in a rolled up state. Right click on the file name and select Send to Compressed (zipped) Folder. Attach the resulting *.zip file here.
steinmini,
Thanks for the star. And there is NO need to apologize for your English, it is very good.
Shaggy's suggestion for two configs, one detailed and one simplified, is a good one. I would suggest suppressing the text at least for the simplified config.
Perhaps you are willing to share your model (you'll get us to take a good look at it and make even more particular tips) or not (likely for proprietary reasons - quite understandable).
I wonder, does your circular pattern 17 cause the multiple bodies? I suspect that it could be causing a slightly mismatched cut and leaving trace bodies that aren't readily visible. If this were cleaned up by preventing the trace bodies rather than adding another feature to remove them you might have a much faster model.
- - -Updraft
Thanks for the star. And there is NO need to apologize for your English, it is very good.
Shaggy's suggestion for two configs, one detailed and one simplified, is a good one. I would suggest suppressing the text at least for the simplified config.
Perhaps you are willing to share your model (you'll get us to take a good look at it and make even more particular tips) or not (likely for proprietary reasons - quite understandable).
I wonder, does your circular pattern 17 cause the multiple bodies? I suspect that it could be causing a slightly mismatched cut and leaving trace bodies that aren't readily visible. If this were cleaned up by preventing the trace bodies rather than adding another feature to remove them you might have a much faster model.
- - -Updraft
CorBlimeyLimey
Mechanical
steinmini ... Take a look at the attached part and compare file size.
I agree with others, posting your part here will allow reviewing and testing on other machines.
I agree with others, posting your part here will allow reviewing and testing on other machines.
CorBlimeyLimey
Mechanical
Ooops, sorry. I attached the unzipped file by mistake, but it's only 1.4MB anyway. (Zipped was .94MB)
- Thread starter
- #17
I started a completely new file. With the text and most of the cuts and shaped edge, the whole file size is around 500kb(SW closed)
I'm going to make a guess now, and might be completely wrong, but as I was toying with this and that solution, I made a whole bunch of "test" attempts within the same file. I deleted the lines/splines/holes/patterns I didn't like, but thought about a possibility that SW somehow "cached" that data and threw it back into my face, resulting with a humongous file size.
In addition, or instead, "Updraft" might be also right, "slightly mismatched cut" is something that happened to me a few times, and even though I deleted it and created a new sketch that resulted with a clean cut, something probably remained that created that 5 extra bodies...
I'm grateful for all the help you guys offer and provide, but I wouldn't bother you with repairing my mistakes, after all, this is not a "to be, or not to be" sort of problem, but a good lesson on a simple example. I'm doing it for a friend in Denmark, (I'm from Serbia) free of charge, for his Intense Kawasaki M1 dirt bike (bicycle), and one day, if time permits, he might return the favor somehow
I downloaded the part file attached by CorBlimeyLimey and I think I already learned something about alternative ways to get a desired shape. Will have to look into it a bit more, but looks very good.
I'm not sure if I may slightly veer off the topic...
when designing the brake disc, two elements are important:
stability (resistance to side flex) and
cooling (excessive heat dissipation)
Stability is achieved with proper thickness and well designed "spokes", heat dissipation with many small holes that increase the surface from which the heat can get away.
So, if you ever get a question from someone (friend or customer) is it possible, keep these two vital features in mind. When I finish the design, I'll upload it and make it available for editing (text, shape, etc) and use, free of charge. I think it's fair enough I'm not making money on it, so it's all the same to me if it's used for two or two hundred pieces (whoever chooses to use it, will have to pay for laser cutting and brushing from his own pocket, though )
I'm going to make a guess now, and might be completely wrong, but as I was toying with this and that solution, I made a whole bunch of "test" attempts within the same file. I deleted the lines/splines/holes/patterns I didn't like, but thought about a possibility that SW somehow "cached" that data and threw it back into my face, resulting with a humongous file size.
In addition, or instead, "Updraft" might be also right, "slightly mismatched cut" is something that happened to me a few times, and even though I deleted it and created a new sketch that resulted with a clean cut, something probably remained that created that 5 extra bodies...
I'm grateful for all the help you guys offer and provide, but I wouldn't bother you with repairing my mistakes, after all, this is not a "to be, or not to be" sort of problem, but a good lesson on a simple example. I'm doing it for a friend in Denmark, (I'm from Serbia) free of charge, for his Intense Kawasaki M1 dirt bike (bicycle), and one day, if time permits, he might return the favor somehow
I downloaded the part file attached by CorBlimeyLimey and I think I already learned something about alternative ways to get a desired shape. Will have to look into it a bit more, but looks very good.
I'm not sure if I may slightly veer off the topic...
when designing the brake disc, two elements are important:
stability (resistance to side flex) and
cooling (excessive heat dissipation)
Stability is achieved with proper thickness and well designed "spokes", heat dissipation with many small holes that increase the surface from which the heat can get away.
So, if you ever get a question from someone (friend or customer) is it possible, keep these two vital features in mind. When I finish the design, I'll upload it and make it available for editing (text, shape, etc) and use, free of charge. I think it's fair enough
I'm not making money on it, so it's all the same to me if it's used for two or two hundred pieces (whoever chooses to use it, will have to pay for laser cutting and brushing from his own pocket, though )- Thread starter
- #18
CorBlimeyLimey
Mechanical
Having trouble extracting that RAR file. Could you repost using ZIP or Windows compressed format.
- Thread starter
- #20
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