Bad Slot, Bad..... No donuts (or Hex Nuts)! 3

[phlyx]

I have seen several ways to make a slot in a part and have no problem with that BUT when you make a slot it's normally for a fastener to reside in (with a washer and lock washer) and thread into a mating hole. When you mate these two parts and then you wish to place the washer, lock washer and bolt, I can't seem to find an easy way to mate the first washer concentric with the tapped hole but coincident with the face of the part with the slot. I end up putting it coincident with the tapped hole (inside the slotted part) and then edit the mate removing the tapped hole face and then selecting the slotted part face.

Anyone have any easier ways of doing this? (Hints also accepted on easy ways to input slots other then sketching two circles, drawing lines or rectangles, trimming out what's not needed and remove extruding)....

Thanks!

~ Phlyx ~

 

[SBaugh]

Don't use the faces (concentric, etc..) Use a plane that goes through the middle of the slot (from the part level). Then you can use a plane from one of the bolts, or nuts, etc... If you make and use the correct plane, the part can still function correctly like a slot is suppose too.

When assembling you should highly consider using planes instead of faces, etc... because planes will always be (unless you specfically delete them) they are unlike faces where if you change something a face can be changed or removed without your knowledge and your mates may fail later in the products life change.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[JahnEng]

The easiest way to make a slot on a single part that I found is to use slot under tools- feature palette - palette fetures - machined... There is also a curved slot. For mating you should consider using scetches. I modify the scetch of the slot by adding a couple of points. These new points will be concentric with tapped holes, screws and washers...
Hope this helps...

Eduard F.

 

[CorBlimeyLimey]

phlyx
As JahnEng suggests, the feature pallettes is probably the best way to go.

However, a method I often use is to drag & drop a sketch from a part which consists of a selection of previously created and often used profiles (ie. No solids). I named the part "Profiles.sldprt" and each sketch within it is named according to its shape (Obround, Star-5 Point, Slot, S, C, etc). I often have the Profiles part open all the time when producing new parts & simply drag the sketch from the feature tree into an open sketch in the new part. The sketch profiles are fully dimensioned but not located on an origin so that it remains free to be located, re-sized & constrained after dropping it into the new sketch.

SBbaugh
If you haven't already, perhaps you should create an FAQ regarding "Good Mating Practices"


CorBlimeyLimey
Barrie, Ontario
faq559-863

 

[aamoroso]

I personally disagree with using planes to mate. Number one if you have multiple users accessing files over a server, a plane can be changed by anyone at anytime. Number two, if you are mating two parts together it is more likely you will want the part to move when the face of it is changed, (ex a cap screw moving when a counter bore is made deeper). Number three, and most important when you go to build the product in the real world the planes are not part of the product, so any interference detection you do may or may not be accurate. For your specific application, I believe you are using some sort of fastener, you can mate the washer to the bottom of the fastener and then the fastener to the hole, and washer to the part it will actually be tightened to.

 

[SBaugh]

Number one if you have multiple users accessing files over a server, a plane can be changed by anyone at anytime.

A mate can be changed just as easy. If a part is changed and the face ID changes, you will lose the mate. You will have to repair it and sometimes it's not to bad especially with the tools that you have today. But if you have changed numerous parts and the face ID's have changed, or you have removed a hole and re-added the hole some where else on the part (then the ID's are totally gone) your going to get a lot of errors in the mated assembly.

Number two, if you are mating two parts together it is more likely you will want the part to move when the face of it is changed, (ex a cap screw moving when a counter bore is made deeper).

If that's the case then you can offset a plane at the part or assembly stage and do an in-contexted relationship so it updates. If you in-context it to a face and the ID changes, then you have a real hassle on your hands. In-contexted repairs are not fun and can get very confusing fast. So if you don't want a lot of problems in-contexting, then Planes are your best bet.

Number three, and most important when you go to build the product in the real world the planes are not part of the product, so any interference detection you do may or may not be accurate. For your specific application, I believe you are using some sort of fastener, you can mate the washer to the bottom of the fastener and then the fastener to the hole, and washer to the part it will actually be tightened to.

You can do the same with planes. Offset 2 two planes from one of the default planes so that it sits on the same face as both outside faces at the part stage. Do this for every part. Then use those planes to mate with at the assembly. What would be the difference if you use those planes versus faces? You wouldn't have to worry about losing Face ID's anymore. You can set up a DT to control placement of those planes in each of the parts so if the thickness changes the planes update, and so on to the assembly. yes it takes more time to do some of this, but the large and biggest benefit is a flawless running assembly. You won't have to worry about as many problems and errors when using planes versus faces. If you use a concentric mate to control the hole and the bolt... what's the difference between using a plane the goes down the center of the hole and the bolt versus the concentric mate... nothing, because a concentric mate is the theoretical middle of the hole and the bolt. Well so are the planes of both parts.

I spent 2+ years doing automation in SW. These are the tricks I have found in my pursuit of a flawless in-contexted assembly. I have built some very large designs and I have informed others of how to do this and they have built larger assembly with my methods and they work flawlessly if you do it correctly. I have one customer that just built a 15,000-part assembly in SW. On top of the size it's fully in-contexted, with a DT and equations. Others use this assembly and as long as they have an understanding not to edit certain parts of the assembly then the assembly will work. They only have to change 3 or so things and the model assembly fully updates to the size. And that is the way I built my in-contexted assemblies when I worked with automation.

You may not agree with me, but you should at least try it out. Also look through this site of mine. There is some information on this there. There is also an article that I wrote on the 1st fully in-contexted assembly mated to and in-contexted to planes only.

http://www.scottjbaugh.com/Design_Portfolio/SW Models DT.htm

CorBlimeyLimey
Thanks! I will try to put something together and post it to the FAQ and probably put it on my site as well.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[aamoroso]

That was a nice post Scott, and I do agree that mating with planes does have an upside. Personally I have over 15 years experience in CNC Machining and Manufacturing management and the single biggest reason I prefer mating to faces is so when our other engineers with less manufacturing knowledge put an assemble together they will get errors and see problems when assembly is rebuilt. If the planes are setup correctly you will achieve the same results, except there you are relying on the planes being setup properly.

 

[SBaugh]

Thanks!

You have to take the time to set the planes up, that's the whole idea. You have to think ahead when building your parts and assemblies in SW. You should do all of this anyway when building anything in SW. SW is built on Design Intent and that should the first thing that anyone does before starting on a project.

I'm sure that most engineers would be able to understand the assembly process once that got a grasp on SW. Once you get that grasp using planes for mating would probably be the better way to go, IMO. Just from personal experience and the errors I have encountered over the years.

The biggest thing I still stress to you and everyone is that when you make changes to parts. It's very likely that you might loss face ID's and when that occurs you lose mates. If you offset the planes using the Default planes (Front, Top, Right) and don't use any part of the geometry your chances of keeping your assembly intact is a lot higher. Also the use of Equations and DT are needed to control placement of planes, especially if you plan on the making the file either in-contexted or larger.

Well I hope the faces work for you and I understand what your saying about using the faces to show the engineers how it works. Just trying to make things easier for you and your colleagues.

Best Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[SBaugh]

CorBlimeyLimey and everyone else that is interested - please see faq559-871 for more information on mating. If you find a problem or something let me know.

Thanks,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[JNR]

Hmmm..... interesting. I see your points on using planes Scott, but I disagree for OUR PURPOSES. We have some pretty strange shaped parts and mates. Anyway, it would be too late for us to change now - it would wreak havok in our PDM system!! Mind you, I don't think there is a single best answer for all purposes on a lot of these issues, is there?

On the other hand, I don't understand the original problem. We have similar parts where the inside bore of the "washer" is mated concentric to the hole in the underlying part, but its face is coincident with the slotted part. It works fine - though you do have to pay attention to the order in which you stack parts up if there are a lot of parts and mate depedencies. Just do it the way they would be physically restrained in practice is best (not necessarily the way you would actually assemble the parts by hand). Note that from our experience, the concentric washer mate should happen first - then the coincident washer mate. THEN I would mate the bolt to the WASHER. If you try to mate the bolt to the hole and the washer face it seems to want to go unstable at times. I know you would not normally assemble this by placing the washer on the slotted surface rather than on the bolt first, but the software likes it better.

Which brings me to another pet peeve. "Rotational parts" like washers, screws, dowel pins and a host of others. You mate them concentric and coincident. Then you have to somehow artifically trap their rotation with another mate just so they are "fully mated". Other wise you get all those darned "-" signs!! Why can't SW give a simple special mate for these things that will (semi)automatically fix their remaining (rotational) degreee of freedom?

BTW: This is how someone here took care of the issue with slots for a while. He put construction entities in the slot sketch for its centerline and a circle concentric with its midpoint and tangent to one side. Then he mated to this. Its a bit messy and reqires some forethought but it did work.

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