I need to pattern every feature in this model except for the base. Selecting all features(except the base) and trying to pattern does not work. I would like to try and make all the features I want to pattern into one feature (solid body) and then try to pattern it. I see commands that say "Delete Solid Body" and "Save as Solid Body" but none that say "Create" solid body. I think I have done this before but can not remember how.
Thanks-
I selected all the features and tried to use the combine command but it is greyed out.
Hello Jody,
As Chris said, the Combine feature should work for you, but I wonder why you couldn't pattern the separate bodies. Is it possible you had the default "Features/Faces to Pattern" selected instead of "Bodies to Pattern"? (See #21 at Frequently Asked Forum Questions.)
Jody Holm wrote:
I selected all the features and tried to use the combine command but it is greyed out.
Is it possible that you only have one body? That would explain why you're having problems with patterning. Can you post the part?
This looks to be just a straight forward feature pattern. I am wondering why "Selecting all features(except the base) and trying to pattern does not work".
Can you share the part? Have you tried the "Geometry Pattern" selection in the feature pattern dialog box?
Glen, you are correct. I did not have "Bodies to Pattern" selected. Actually, I thought you had to create a body before you had a body...which I did not do. However, as you stated, the whole model wants to pattern when I do what you are saying. Could the reason be that the 2nd feature is merged to the base? Bad news is, when I un-murge it, a bunch of other features fail.
Dan, I did all that "Geometry Pattern" flip flopping with no luck.
Jody,
Any time you create any solid geometry (with Extruded Boss/Base, Revolved Boss/Base, Weldment, etc.) you create a body. As you add material you're either creating new, separate bodies, or adding material to the original body by choosing the "Merge result" box in the FeatureManager. It sounds like you have that part figured out. I can't diagnose why you're getting errors without seeing the file, but you'll likely just have to fix them (or if you'll post it here I'll try to help).
Glenn
Hi Jody,
I have to go with Glenn's assessment.
When creating the features to be patterned, be selective in regards to Feature Scope so that the newly created bodies are not combined with the base. In other words be sure the base feature is NOT included in your Feature Scope as your create the new features. (Boss-Extrude1 being the base in my example here)
Then make your pattern of bodies as suggested by Glenn.
Finally, used Combine to make it into one solid body for production.
I hope this helps!
James
It looks like it might have something to do with a patterned feature (4 humps) that I am trying to include in my overall pattern. Gotta run. I'll try again tomorrow. Thanks
James,
What you are suggesting is completely correct. One minor thing I am wanting to add for original posters clarification is that the 2nd feature needs to have merge results turned off. This is due to the fact that until you have at least 2 bodies feature scope does not appear.
~Eric
Correct Eric, I did bypass that detail.
Feature Scope dialog is not offered until after multiple bodies are existing. Until then, only the check box to Merge/Not Merge result, the desired option being to Not Merge. I would hope the verbal explanation above might have sufficed, but thanks for pointing out the gaffe.
Jody,
The first feature created after 'base' is completed should not be merged! ;-)
JKH
OK. I'm back. It appears that Dans "straight forward" feature pattern command is the way it should be. I've done many models, many, many times with no regard to the second feature being merged....which by default, it always is. I have attached the file. If this merge thing was true, I would not be able to pattern the first 9 features...which I can. The problem appears to be patterning a pattern, which I have also done many times. Also, I'm on SW14 and I don't see those check box's you mention (red arrow). Here is the file. Give it a try.
I guess this post was "How to make a Solid Body". So, the merge stuff is probably required for that. My real problem was gettting the pattern to work. I ended up patterning the the first 9 features then adding the remaining features one by one to the pattern. Then I had to add the last 3 features to each patterned instance to get everything in. Pretty round about way to do something seemingly simple, but we press on. Thanks for all your help.
Hello Jody,
I got it to work okay. I did get a few errors, but they were easy to fix. I don't have SW2014 loaded so I did it in SW2016, but you shouldn't have any problems. I started at the bottom with each Boss-Extrude, edited them, and un-checked the "Merge result" box. The Fillets threw up errors, since you can't use the feature to fillet between two separate bodies, but ignore that for now. Now backtrack and re-edit the other Boss-Extrude features, starting with Boss-Extrude3, re-checking the "Merge result" box and choosing which bodies to combine at bottom. (Auto-select will likely be checked at bottom by default. De-select it and you'll be able to choose which bodies to combine from the graphics area.) At some point you'll get an error in Cut-Extrude2, because it thinks you want to cut the base. Edit the feature, de-selecting it at the bottom and choosing the other, smaller body. As you work your way down, re-combining the small bodies, the Fillet errors will go away on their own. After you finished that you can create the Linear Pattern without any problems. Just remember to select "Bodies to Pattern".
I hope this helps.
Glenn
Jody,
Glen is correct, you have to pattern body.
First, split the part into two separate bodies, base and shape.
Second, pattern the shaped body.
Third, combine all bodies.
Thanks Glen. Creating a solid body as you described did allow me to create the pattern. I guess it would have been much easier if I had created the base last and un-merged in this case.
Jody Holm wrote:
I guess it would have been much easier if I had created the base last and un-merged in this case.
Nothing wrong with creating the base first. It was that default "Merge result" in the first small Boss-Extrude that got you into trouble. If those first two bodies hadn't been merged from the start you could have merged all the other small bodies as they were created and you would have been fine.
OK, I got it to work with a simple feature pattern.
I create a linear feature pattern and first ONLY selected your second extrude. That worked just fine.
Next, I edited the pattern and added in the Fillet2 (the 3rd feature in your tree) and that worked.
I started walking through your tree, adding each feature one at a time and testing it out, then going back and editing the pattern and adding in the next feature.
The first error that I ran into was LPattern1, but I got this to work just fine by editing LPattern1 and unchecking "Geometry Pattern" and continuing.
The second error that I ran into was Draft4. For some reason, that just didn't want to pattern. So instead, I deleted Draft4 and Fillet7 and embedded them into Boss-Extrude5 (in order the make the same features, I had to offset the sketch plane by .35" and extrude the opposite direction down to the base of the part, I added draft into the extrude and added the fillets into the sketch itself).
This took care of that error. See screen shots below.
After that, the pattern worked great. I will attach the file, but I saved it in SW2015 (I don't have 2014), but the screen shots should be able to help you.
I didn't need to pattern separate bodies at all. It was just figuring out how Solid Works likes it handled. I don't understand why Draft4 didn't want to pattern, but making the same exact feature in a different way fixed the problem.
So you were correct about patterning the pattern being the problem Jody. I tried to pattern just the features and got an error about geometry pattern needing to be unchecked. Since it wasn't checked in the pattern I was trying to create I realized it had to be in the pattern I was trying to pattern. I unchecked geometry pattern in Pattern1 and now the only thing I couldn't pattern was the Draft4 at the end, and thus the last two fillets 8 and 9.
Right on. That's exactly the way I ended up having to do it. I had to add the last draft and the 2 last fillets individually to each instance. Thanks!
I did the same as Glenn except I rolled it back & started at the top.
1. 'Un-merge' Boss-Extrude1 (mold) from Boss-Extrude2 (base) to create 2 solid bodies. See Solid Bodies folder at top of tree. The folder should show up automatically when you have more than 1 solid body.
2. Redefine all the Boss & Cut-Extrude features below that, using Feature Scope to merge (or cut) only the mold body. The new solid body will by default take the name of the last feature created, hence the Draft1 to Boss-Extrude3 naming (you can also name them if you prefer and they'll stay as named, sometimes handy). You can populate the Feature Scope dialog window by picking in graphic area or from the Solid Bodies folder. LPattern1 will also need the Feature Scope defined to merge only to the mold & not to the base.
3. When you get all the additive/subtractive features edited for Feature Scope you should have 2 solid bodies.
4. Create LPattern2 using bodies rather than features. You end up with 17 solid bodies- 1 base, 16 molds.
5. Finally use the Combine tool to make it back into a single solid body and voila, ship it! (Insert > Features > Combine)
I composed this earlier & my internet connection failed before I posted, *%&^$%(&^!!!...!
Sorry if my step by step illustration seems a bit elementary, I just want to be sure it communicates clearly. If there are questions or I left something out let me know.
Of course there's a hundred ways to skin this cat, you could probably not merge anything until the final Combine command etc. etc..
I'm not expert enough to know why SolidWorks sometimes rejects feature based patterns but I think you're on to something with you're suspicion of LPattern1 as the culprit. If you do a lot of mold/cavity type work though I think you'll find that multi-body parts are your friend.
Best,
James
Did you see my post from above? If you change how the draft is done, you can run a feature pattern (without extra bodies) on this no problem, including the draft features and still get the exact same result. Also, it gives you a smaller feature tree (less steps) overall.
And because I'm a geek...
A couple more features and you have your molds. You can have your core(s) and mold parts as configurations of a single part document, very convenient.
1. I Shelled your model (the back & side faces of the base) to .010" to create a core
2. I mid-plane Extruded a rectangular block encompassing the core, unmerged. (nearly encompassed...real world design would require a different approach)
3. Use Combine tool to subtract the core, leaving upper & lower mold halves. (Hence nearly encompassing the core- I wanted the Combine/Subtract feature to result in 2 bodies. You can figure this out for real world use as you wish...)
4. The Body-Move/Copy feature is only for the snapshot.
I know very little about molding so sprues, risers, ejection pin bores or whatever else you need for the real world is your deal...
I hope this helps you.
James
Whatever gets the job done right!
I'm sure I should so leave it alone but in my humble opinion acclimating to the 'to merge or not' question seems easy & routine as compared to analyzing/diagnosing/repairing drafts & other features after they are created (no offense to Dan or Sarah, whatever gets the job done is good). Patterning bodies seems to be a lot less picky about the complexity of the features within and (so far) works every time for me. I hope you at least will experiment with multi-body parts and form your own opinion. My $0.02 worth for ya.
Cheers,
JKH
Oh no! I agree. It is just that, for me personally, I tend to prefer using a single body without combines if at all possible. But, failing that, multi body parts are definitely the way to go.
It is just a personal preference. One of those quirks we designers are known for.
Have you tried the Combine command?