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Fillets in machining 2
- Thread starter sudhakarn
- Start date
-
1
- #4
IrishMariner
Aerospace
Hi,
Your question could be either "What fillet radii should I use" or "How do I add fillets to a part I model in V5"
If it's the former, and it's metal parts you are working with, There's lots of design guides on the internet, eg:
The corner radius/ fillet radius is normally dependent on the feature being manufactured and is a trade-off between machining speed, tool stiffness, component weight, etc, etc. for example, a small corner radius means a small cutter will be needed so it will take longer, but a larger cutter might make a part too heavy. Similarly, a deep pocket traditionally demanded a corner rad ~1/4 the depth or more, but nowadays machine shops can break this long time 'golden rule' with high-speed machining or using z-plunging. Fillet radii can be selected based on standard tooling (so that a custom cutter isn't needed) and might need to be a certain size for stress reasons too.
If the component is plastic, then fillet radii is dependent on a different set of conditions (and I know nothing about plastic)
Long story short, you should consult your manufacturing engineers who will advise.
If your question is about 'how' you fillet a part in V5 then you have choices. It can be done by either:
1) Using the Part Design fillet command in 'Dress-Up' ( the preferred way I expect)
2) if you are using surfaces to shape the part body then an edge fillet or shape fillet on the surface from GSD can do it. I sometimes use 90deg circle surface from the 'swept surface' menu and the 'limit curve and tangent surface' option.
3) For parts such as wing skin machinings that are machined using compound cutters that have different radii, then I sketch the profile of the cutter and sweep it along a curve that represents the shape of the pocket. I split the body with the resulting surface.
I sometimes use Boolean solids for complex machined parts (and I often hear this is wrong but I've yet to hear a good reason why) and in this case I just fillet the body being removed.
A couple of v5 filleting tips I will pass on:
1) When you begin a model, add a parameter or two for 'Corner Radius' and 'Fillet Radius' so that you can swiftly make changes later if you get advised to do so. Also, in my experience of modeling aerospace parts, the chosen radii can affect positioning of fastener locations or other features so a parameter allows them to be referenced.
2) The order in which you fillet edges in a model is important. An incorrect sequence can result in either a failure to fillet or, worse, an unrepresentative result. Either way, experience is your friend and trial and error your path to experience.
3) Fillets do not belong in sketches. They just don't.
I've found it better to have them as features in the part body spec tree. One reason being that it's easier to deactivate them if a stress engineers wants them off for an FE model, or you need to create a 'mid-surface' model.
Good luck
Your question could be either "What fillet radii should I use" or "How do I add fillets to a part I model in V5"
If it's the former, and it's metal parts you are working with, There's lots of design guides on the internet, eg:
The corner radius/ fillet radius is normally dependent on the feature being manufactured and is a trade-off between machining speed, tool stiffness, component weight, etc, etc. for example, a small corner radius means a small cutter will be needed so it will take longer, but a larger cutter might make a part too heavy. Similarly, a deep pocket traditionally demanded a corner rad ~1/4 the depth or more, but nowadays machine shops can break this long time 'golden rule' with high-speed machining or using z-plunging. Fillet radii can be selected based on standard tooling (so that a custom cutter isn't needed) and might need to be a certain size for stress reasons too.
If the component is plastic, then fillet radii is dependent on a different set of conditions (and I know nothing about plastic)
Long story short, you should consult your manufacturing engineers who will advise.
If your question is about 'how' you fillet a part in V5 then you have choices. It can be done by either:
1) Using the Part Design fillet command in 'Dress-Up' ( the preferred way I expect)
2) if you are using surfaces to shape the part body then an edge fillet or shape fillet on the surface from GSD can do it. I sometimes use 90deg circle surface from the 'swept surface' menu and the 'limit curve and tangent surface' option.
3) For parts such as wing skin machinings that are machined using compound cutters that have different radii, then I sketch the profile of the cutter and sweep it along a curve that represents the shape of the pocket. I split the body with the resulting surface.
I sometimes use Boolean solids for complex machined parts (and I often hear this is wrong but I've yet to hear a good reason why) and in this case I just fillet the body being removed.
A couple of v5 filleting tips I will pass on:
1) When you begin a model, add a parameter or two for 'Corner Radius' and 'Fillet Radius' so that you can swiftly make changes later if you get advised to do so. Also, in my experience of modeling aerospace parts, the chosen radii can affect positioning of fastener locations or other features so a parameter allows them to be referenced.
2) The order in which you fillet edges in a model is important. An incorrect sequence can result in either a failure to fillet or, worse, an unrepresentative result. Either way, experience is your friend and trial and error your path to experience.
3) Fillets do not belong in sketches. They just don't.
I've found it better to have them as features in the part body spec tree. One reason being that it's easier to deactivate them if a stress engineers wants them off for an FE model, or you need to create a 'mid-surface' model.Good luck
- Thread starter
- #5
A fillet is typically a concave inside corner blend between two adjacent surfaces. Fillets can have a radius profile or an elliptical or conic profile shape. The exact method for producing the fillet surface will depend on the manufacturing process used to produce the part. If a part is cast then many of the fillets will be produced as part of the casting. If the part is machined then some small fillets will be produced by the shape of the cutting tool edge, and larger fillets will be produced by the path of the cutting tool.
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1
- #7
Hi,
Regarding boolean operations and fillets in V5:
I worked on many part which were designed in V5 especially some really complex ones which are used in JSF. Sometimes fillets look like a mess. But we NC-programmers are tough as nails and make it. However, if an engineer lacks surfacing skills then the design is unnecessarily complex or sometimes these new engineers only know a little about creating a sketch and then create a solid and then cut a pocket, boolean, etc.. No offense but we are missing the talent in the aerospace manufacturing industry.
Last year I worked with another customer and helped their engineers to make a proper run-out radius for cutting a chamfer. And I made a UDF for them in V5 with parameters such as Tool-Dia, Tip-Dia along with other lengths, and angles for the chamfer. It's not only these parameters, the main thing is how deep I will push the cutter so its tip is below the chamfer edge which will change the shape of cone at the run-out. An experienced NC-machinist and NC-programmer know how exactly it will be made so it is natural for them to come up with such ideas and store in V5 UDFs or Powercopies for the future reuse for any tooling design.
Nowadays, the main problem is lack of machining education provided in the schools/colleges. Anyway I don't want to derail this thread completely but it becomes touchy when an NC-programmer have to work on somebody's designs and the designer doesn't have sufficient info regarding how it will be manufactured.
I often say and preach that the first NC-Program for any machined part is a Blue-Print or an Engineering-Drawing made by engineer/designer.
Here is one important tip for the new generation of engineers. Whenever in doubt how to make some design feature such as fillets or anything, just ask yourself how did someone make it when there was no cadcam around. It will fire up a reaction in your mind and will compel you to find your answer/solution on your own. Then you might be able to decide if you can make an old idea better and more efficient with today's new technology. And there is nothing new. It has been done and made before by our ancestors many times over and over. Most of the times we fail to realize it.
peace..
SSC
Regarding boolean operations and fillets in V5:
I worked on many part which were designed in V5 especially some really complex ones which are used in JSF. Sometimes fillets look like a mess. But we NC-programmers are tough as nails and make it. However, if an engineer lacks surfacing skills then the design is unnecessarily complex or sometimes these new engineers only know a little about creating a sketch and then create a solid and then cut a pocket, boolean, etc.. No offense but we are missing the talent in the aerospace manufacturing industry.
Last year I worked with another customer and helped their engineers to make a proper run-out radius for cutting a chamfer. And I made a UDF for them in V5 with parameters such as Tool-Dia, Tip-Dia along with other lengths, and angles for the chamfer. It's not only these parameters, the main thing is how deep I will push the cutter so its tip is below the chamfer edge which will change the shape of cone at the run-out. An experienced NC-machinist and NC-programmer know how exactly it will be made so it is natural for them to come up with such ideas and store in V5 UDFs or Powercopies for the future reuse for any tooling design.
Nowadays, the main problem is lack of machining education provided in the schools/colleges. Anyway I don't want to derail this thread completely but it becomes touchy when an NC-programmer have to work on somebody's designs and the designer doesn't have sufficient info regarding how it will be manufactured.
I often say and preach that the first NC-Program for any machined part is a Blue-Print or an Engineering-Drawing made by engineer/designer.
Here is one important tip for the new generation of engineers. Whenever in doubt how to make some design feature such as fillets or anything, just ask yourself how did someone make it when there was no cadcam around. It will fire up a reaction in your mind and will compel you to find your answer/solution on your own. Then you might be able to decide if you can make an old idea better and more efficient with today's new technology. And there is nothing new. It has been done and made before by our ancestors many times over and over. Most of the times we fail to realize it.
peace..
SSC
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