To make a long story short when we have castings we will insert the casting part into an assembly. Then add assembly cuts to make the machining. I could save a lot of time making new configurations if I could add material.
If I want to make a drawing of an as-cast part and another drawing of an as-machined casted part, then I will insert the as-cast part file into a new, as-machined part file (not into an asembly file). I need no configurations.
Why insert into an assembly? Why use configurations? Why do you want to add material when machining a casting involves only material removal?
I guess I need you to tell the long story.
We had looked at inserting the casting part into a machine part or assembly. We decided to go with an assembly. I do not remember all the reason why we went this way. One of the reasons is on the drawing we can insert a BOM and have the casting and heli-coil inserts show up. With all the limitations I have ran into using assemblies as my machine part it might have been better to go the insert part into part route but that is a different conversation.
I have an existing machining part I want to add a 02 configuration to. The 01 configuration has a grove cut in it that I don’t need but instead I need it to extend out. If I could add an extrude revolve to fill in and add what I need, it would take about 2 minutes. The casting has the material to do this so in the end in still removing material.
Instead I had to suppress the cut revolve that made the grove. This in turn suppressed 4 other features. I then had to add a new cut to make the extended part and add the other features that were suppressed. This took around an hour.
I know that if the grove was a feature by itself that would have made things a lot easier. This casting was made a few years back and was never intended to be used in any other place but things change.
As far as adding a configuration or making a new part number again that is a different conversation.
In the end it really comes down to saving time and not why I’m doing it.
If you can, post an image or preferably the part itself, someone may be able to offer a better method.
I’m guessing there are 20 different ways I could have done it. Over the weekend I thought of a better way I could have done it but it was too late already done.
I’m not looking for different ways or even why I’m doing it. I want to know if other users would find it useful and save them time. If so I’m going to create an enhancement request and try to get people to vote for it.
I want to know if other users would find it useful and save them time.
Don't worry about whether others would find it useful. If you would find it useful that's all that really matters. Submit the ER.
However, I would not use that function (for the type of fix you specified) but I'm sure some others would. IMO, the only material additions at the assy level should reflect those which can be applied in real life. (welds, spray-on or dipped coatings, etc). In real life material cannot be machined on to a part.
When I do castings, I make a casting model and drawing. I attach the casting model to an assembly, and I make the machining drawing from this. At this assembly level, all I can do is remove material, but this limitation exists in the real world, too. In the assembly model, I can add thread inserts and dowel pins, just like in the real world.
When I design machined parts, I define the primary outline, then I remove material. I never add material to a machined part. Machinists cannot add material either (without welding). When you design stuff, you need to keep aware of how the fabrication process works. Just because SolidWorks can do it, don't assume it will happen in the real world.
If I want to add material to the casting, I need to add it to the casting model so that it is reflected on the drawing and/or model that goes out to the foundry. If you want to weld stuff to a casting, you can do this at the assembly level.
A big frustration of mine with SolidWorks is that people out there will create what they want in the model, and disregard the process of ordering the designed part. If you add material to a casting at some subsequent assembly level, this modification will not be seen by the foundry. We need to order parts! Your modeling must support an ordering process of some kind.
I do castings the same why as you do. I have a casting that has a good inch of material in one spot being cut away. Since I have so much material I can use this for a different job. I’m still removing material from the casting in the real world.
Because the part was not setup in the beginning to make this type of change it took a lot longer to do. If I could of filled in the grove and then add the bump I would have been done in 10 minutes.
Also I would have loved to add material to an assembly when I was doing concept designs that I knew would never be used for manufacture.
Are you making two different parts from the same casting? This is not a problem. Make two machining drawings and assembly models. Cast the bump in place, always. When you want a slot, machine it out.
Your procurement will see one casting, and two machined parts. Remember, machined parts are easy to revise. Castings are expensive and complicated to revise, however easy it is in SolidWorks.
At preliminary design time, I create a blob to represent the final assembly. This shows the overall configuration of the system. I can add material if I want because the blob is a figment of my imagnation. As I continue designing, I populate the blob with real components in which I follow my design rules, above. When I have everything figured out, usually, I delete the blob.
Yes I’m making two different parts from the same casting. The casting was made 2+ years ago. Original part had 1” cut down, then a ¼” slot. I want to make a part that I cut down ¾” and then 1” everywhere else. Because of how the sketch was made 2+ years ago I can not easily change the shape of the sketch to what I need.
If I did a saves and gave it a new part number I could then just delete stuff I don’t need in the sketch and change it to what I need. I don’t have the option.
Are you allowed to modify the casting? The real, physical casting requires somewhere between five to twenty thousand dollars investment, and perhaps even more. Almost certainly, you are not allowed to modify it. You can add material either by welding, or with screws or adhesive, at the assembly level.
Possibly, the casting has been modeled badly, and SolidWorks does not reflect what comes from the foundry. In this case, you need ot go back to the casting model, and fix that, and the drawing attached to it.
You could add material by attaching a part to your casting, and excluding it from the BOM. This will accomplish your purpose. It also will ensure that the next person who has to work on this thing will be even more confused than you are.
You should not be operating SolidWorks. You should be doing mechanical design, using SolidWorks as a tool.
I have attached an example of what I’m trying to do. This is just a real quick example.
Now I see what you are doing.
My suggest above will work. My comment that goes with it still is correct.
I think it would be easier to modify the -01 configuration to show the extra material, and add an additional cut to -01 to remove it. Machinists cannot add material. Your model should work that way.
In that example that is how I would have done it.
I always take into account how it’s going to be made in the real world and your right machinists cannot add material.
Now that you see what I’m doing would you find it useful to be able to add extrudes in assemblies? Don’t think of it as adding material.
My point of view is just because you can’t do it in the real world I should still be able to do it in the software. Yes you can screw things up real quick and design stuff that can’t be made. I don’t think the software or tool I use should be limited because of it. Just my two cents.
Without getting into the debate about why you are doing what you are doing etc. etc.
I got thinking about what you are trying to do and remembered that assembly cuts can now be propagated to the part. If you are on 2012 (maybe possible earlier, I don't remember when I first found it) you might try that until your ER is granted.
The option to propagate to the part level is when you are editing the feature in the assembly. Also, in the part you can make the feature independent if you need to.
If you can propagate the groove you want to fill up to the part, then open the part and fill it in, back in the assembly the dependent assembly features should still be OK.
I'm out of lunch time right now, but I made a quick test with a part in an assembly. Made assembly cuts propagated to the part, threw in some dependent features here and there and filled the cuts at the part level. I don't think it's much more (if any) work and time than making the "fills" in the assembly itself would be. See if it makes sense to you.
It sounds like your assembly has gotten kind of complicated over time so this may not be a workable option for you.
An assembly by definition does not have material. So, you can not add material. An assembly is a collection of parts mated to positions. If you want to add "material", you would need to add parts. You have to think about an assembly as a mechanism (skeleton) linking all components together. An assembly by itself is "empty" in nature. If you think about it this way, you would not want to add "Material".
I hope this helps!
Thank you for not debating why I want to do this.
I just got home and will take a look at this in the morning. Off the top of my head I don’t know if it will work. I can not change the part because it is a casting. Again thank you for the ideal and I will most defiantly try it.
At home and tried it with 2010. Behavior can be odd. 2012 seemed a bit less so.
My advice based on a not very controlled bit of experimenting:
Make sure you have everything backed up well. I got into a couple of blind allies that I couldn't back out of.
Only propagate the features you need to "undo" at the part level.
Don't make the feature independent at the part level. That really goofs things up.
It's probably too late for your assemblies, but if you knew you were going to be playing this game from the start, make sure you propagate any features before making later ones dependent on them.
Be prepared for dangling dimensions and/or sketch planes etc. They may, or may not be, fixable in the "usual" manners.
It seems more like working with features created in the context of an assembly that has changed than features in a part that changed. Relationships dangle or break but the feature may lock and still remain viable. If you're willing to ignore the unhappy relationships.
As I'm sure you realize this is not something you really want to do if you have any better alternatives. I have encountered more than a few parts and assemblies that were way out of hand but which couldn't be practically tossed and done over (there's this thing called a clock where I work you see). Sometimes you have to just do whatever you can to make it work for you, until that extra time we're all waiting for finally gets here. Then we can all go back and do all those things we're hoping no one notices for now "the right way".
Thanks for the input. I don’t think I want to do that for this instance but it gave me some ideals were else I could use it.
I see your point from a sheet metal reference and how I would have done it from there.
I have one recent part file with seven configurations and seven assembly configurations before I start making drawings. I always use assemblies in drawings, almost never parts. That way if I add a PEM nut into a part I am not presented with an empty drawing sheet or starting the drawing over again. I'm sure we've all seen the empty boxes!
When I was doing sheet metal I had to learn the hard why to always make sheet metal parts assemblies because of pems. I knew for sure this part would never have pems in it but as soon as I finished the drawing I had to add pems.
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