[Larry Dickman]

I'm fairly new to SW, and this is something I haven't figured out how to do. As an example, I draw an arc with a 1" dia at 0,0, and another arc with a 1" dia at 1.375, .375

Now, I want to draw a .250r fillet between them. When I try to do it, SW gives me an error saying the 2 arcs don't intersect.

I can do it in Mastercam or Autocad, and it's a no-brainer, it just does it.

This is something I need to do a lot, mainly in pockets with curved walls. I can get it to work by figuring out the arc center for the fillet, but that's time consuming and needless. Is there some other function I'm not aware of to do this?

TIA

[beege]

If it were me (I don't know Solidworks), I might create a circles .250 larger than the two original arcs, and draw a .250 circle at their intersection, and it would be tangent to the two other arcs. Other than that, a fillet between the two arcs should work.

[Mike 1948]

I'm fairly new to SW, and this is something I haven't figured out how to do. As an example, I draw an arc with a 1" dia at 0,0, and another arc with a 1" dia at 1.375, .375

Now, I want to draw a .250r fillet between them. When I try to do it, SW gives me an error saying the 2 arcs don't intersect.

I can do it in Mastercam or Autocad, and it's a no-brainer, it just does it.

This is something I need to do a lot, mainly in pockets with curved walls. I can get it to work by figuring out the arc center for the fillet, but that's time consuming and needless. Is there some other function I'm not aware of to do this?

TIA

You will have to draw in the .250r arc near were you want it and add a "Tangent" relation to the other 1" dia arcs. Kind of a PITA. OR

This is hard to explain, its kind of a hidden function. Use the line command
1. make a straight line
2 release mouse button leave cursor on line
3. push down button and drag cursor back down the line, then drag out in a circular motion off end of line.
4 You should get a arc.
5 repeat #2 and #3 on the arc.
6. do #5 on the arc

You will have to go back and dimension them.
It takes a bit to get used to.

Mike

[mcarvey]

I'm still a little unclear of what you are trying to do but I took a guess and posted some screenshots that may be helpful. Anytime I make a filet/round in a sketch I like to make a circle, and then connect it to something else via a tangency relation, and then I trim off the unused section (trim-to closest). I'm used to an older version of SW which had some issues, and this is a method that I had success with so I stuck with it.
Was my guess correct or are you trying to do something completely different?

-Matt

[Larry Dickman]

Thanks for the replies. That's exactly what I was trying to do. Seems like a lot of extra steps though. I might have a pocket with all curved walls, and 30 or so fillets. Seems like a PITA, I was hoping there was an easier way.

I guess what I really don't understand is why the fillet function won't do it. If Mastercam could get it to work, it can't be too difficult.

[Mike 1948]

Thanks for the replies. That's exactly what I was trying to do. Seems like a lot of extra steps though. I might have a pocket with all curved walls, and 30 or so fillets. Seems like a PITA, I was hoping there was an easier way.

I guess what I really don't understand is why the fillet function won't do it. If Mastercam could get it to work, it can't be too difficult.

Maybe it would be faster using the "Feature" fillet routine after putting in the rough pocket, instead of the "Sketch" fillet before pocketing. I usually stay away from sketch fillet if possible. The "feature" fillet has more power and less mouse clicks overall.

Mike

[Larry Dickman]

Maybe it would be faster using the "Feature" fillet routine after putting in the rough pocket, instead of the "Sketch" fillet before pocketing. I usually stay away from sketch fillet if possible. The "feature" fillet has more power and less mouse clicks overall.

Mike

Only problem I see there, if I have a number of non intersecting circles that make up the pocket walls, I don't have a chain that I can extrude.

[cygnus x-1]

Only problem I see there, if I have a number of non intersecting circles that make up the pocket walls, I don't have a chain that I can extrude.

I think I see what you're trying to do, and it makes me wonder if maybe it might be easier to define your pockets differently. Is there a simple example part you can share that has a fully defined pocket the way you want it? It would be easier to suggest alternatives if we could see an example.

I'm no SW expert, but if there's one thing I have learned, it's that when something seems more difficult than it should be, there is always a better way to do it.

One possibility is to draw an endpoint arc from one circle to the next, then add tangent relations and dimension.


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[Larry Dickman]

I think I see what you're trying to do, and it makes me wonder if maybe it might be easier to define your pockets differently. Is there a simple example part you can share that has a fully defined pocket the way you want it? It would be easier to suggest alternatives if we could see an example.

I'm no SW expert, but if there's one thing I have learned, it's that when something seems more difficult than it should be, there is always a better way to do it.

One possibility is to draw an endpoint arc from one circle to the next, then add tangent relations and dimension.


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Here is a simple example. The first pic is a view of the pocket. The second view is the geometry. The geometry in green are the arcs and lines that are defined on the b/p. The geometry in red are fillets in between them all. This was drawn in MC. I drew all the Green features, then added the fillets. 2 mouse clicks per fillet is all it takes, no extra geometry, no trimming, just click around the chain and it's done.

[BanduraMaker]

Use the offset entity using the initial set of holes as the source to begin creating your pocket. You should then have mostly intersecting arcs between which you can fillet.

The big benefit to doing that is that if you change the diameter of your holes, the pocket will update automagically.

[cygnus x-1]

Here is a simple example. The first pic is a view of the pocket. The second view is the geometry. The geometry in green are the arcs and lines that are defined on the b/p. The geometry in red are fillets in between them all. This was drawn in MC. I drew all the Green features, then added the fillets. 2 mouse clicks per fillet is all it takes, no extra geometry, no trimming, just click around the chain and it's done.

Interesting part. My first thought (as an engineer) is, do to the pocket walls really have to be that complicated? But it sounds like you are working with someone else's part, so that doesn't really help you any.

The way I would probably approach this is to create offset circles for each of the defined holes. Then sketch in the fillet arcs, and add tangent relationships and dimensions. Then use the trim tool to clean up.

It seems this is one of those occasions where MC has a specialized sketch tool (among many others) that just happens to be perfect for the job. Whereas Solidworks takes a simpler approach with fewer sketch tools that are more universal. It makes sense in that SW is geared toward 3D modelling, where MC is based on 2D sketching. Personally, having learned both MC and SW at the same time, I found that SW is far more friendly and "fun" to use, where MC always seems a chore. But, I digress.

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[Larry Dickman]

Thanks to all for the suggestions. It appears that drawing the fillet arc, then making it tangent to the other arcs is the way to go.

So far, Solidworks is the only cad program I've used where this was an issiue, I'm just curious why. Maybe because they want you to define relationships between all the elements in the chain?:wee:

[SirDenisNayland]

I wouldn't say mastercams tool is specialized.. you select fillet and your rad and as long as the arc can for between two points MasterCAM throws it in there. No special setting, nothing.

There are times however, say creating hose barbs with rads on the "tips" of the barb where I must first create the radius arcs and then join the lines tangent to them, because if I create the lines and then use a fillet, the dimension is altered (diameter becomes smaller).

I think it would be wise when learning any new software to try and forget what else you know, because no program is going to be the same and you'll save yourself the headache of "why doesn't this work, it works in this program!

[cygnus x-1]

I wouldn't say mastercams tool is specialized.. you select fillet and your rad and as long as the arc can for between two points MasterCAM throws it in there. No special setting, nothing.

When I say specialized, I'm talking more about how the interface presents itself. In SW there are 3 arc tools, centerpoint, endpoint, and tangent. Then you rely on relationships and dimensions to define the rest. In MC there are 5, one of which is tangent arc, which has a number of different subtypes. I always seemed to have a hard time figuring out which tool I needed to use for what situation.

There are times however, say creating hose barbs with rads on the "tips" of the barb where I must first create the radius arcs and then join the lines tangent to them, because if I create the lines and then use a fillet, the dimension is altered (diameter becomes smaller).

Actually in that case it might be easier to dimension the outsides of the barb fillets directly. You can dimension the distance between the outsides of circles or arcs by holding down the <shift> key before placing the dimension. So that would be: select dimension tool, click on first circle, click on second circle, hold <shift>, click to place dimension. Not holding down <shift> of course dimensions the center points.

I think it would be wise when learning any new software to try and forget what else you know, because no program is going to be the same and you'll save yourself the headache of "why doesn't this work, it works in this program!

That's very true. My boss learned CAD with Autocad (R12 or so) and more recently learned SW. Early on he was always complaining about how he could do things so much faster in AC, and why can't I do XYZ in SW? And I had to keep explaining that you can't do things the same way as AC because it's not AC. SW is parametric, so while it may take a little longer to create a model at first, it's a whole lot easier to modify once it's created.



Anyway, I was messing around a bit with the SW sketch fillet command, and sure enough it won't sketch fillets to arcs. And arcs can't seem to use the tangent snap either which does seem a bit odd. You can use the "perimeter circle" tool to create a circle tangent to two existing circles/arcs. Then for trimming there is the "power trim" tool where you just click-and-drag the mouse around to delete entities instantly. It's much like using a power hedge trimmer.


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[SirDenisNayland]

Cygnus, what I do is what I believe you described, dimension the outside of the barb fillets directly and then join the lines tangent. Say I have barbs points at x.3 and z-.15,z-.305,z-.360 (yes theyre not all even because they rarely are according to drawings ive found!). what I do when creating any 2d geometry is I sketch my parallel and horizontal lines to get my points. When I have my points at dia. x.3, z-.15 and so on, I create an arc (size of the rad) tangent to two points and voila I have my arc with edges lying on x.3z-.15 and so forth. I then take a line from the bottom of the barb diameter and draw that tangent to the arc and I have the angles. A little trimming and its done. What I used to do (and wrongly, even though really its a hose barb and .001" outside difference isnt going to do jack), was just create the angled line directly to the point x.3z-.15 and then fillet it, which would make the outside edge .2991 or something to that effect.

And this has nothing to do with solidworks so i'll casually leave this thread now!

[cygnus x-1]

Cygnus, what I do is what I believe you described, dimension the outside of the barb fillets directly and then join the lines tangent. Say I have barbs points at x.3 and z-.15,z-.305,z-.360 (yes theyre not all even because they rarely are according to drawings ive found!). what I do when creating any 2d geometry is I sketch my parallel and horizontal lines to get my points. When I have my points at dia. x.3, z-.15 and so on, I create an arc (size of the rad) tangent to two points and voila I have my arc with edges lying on x.3z-.15 and so forth. I then take a line from the bottom of the barb diameter and draw that tangent to the arc and I have the angles. A little trimming and its done. What I used to do (and wrongly, even though really its a hose barb and .001" outside difference isnt going to do jack), was just create the angled line directly to the point x.3z-.15 and then fillet it, which would make the outside edge .2991 or something to that effect.

And this has nothing to do with solidworks so i'll casually leave this thread now!

Not exactly what I was thinking of (if I'm understanding you correctly).

What I meant was to sketch the shape of the fitting first without fillets, just lines. Then dimension everything but the diameter. Then add the fillets at whatever rad you want. Then dimension the diameter from the outsides of the fillets to the center (I'm assuming we're doing this as a revolved base). Here's a screen shot for illustration:




This is obviously exaggerated for visibility, but look at the dimension on the right that sets the fitting diameter (radius actually). I used no construction geometry or trimming to do this.

You're right though. This is getting off topic though so we should probably leave it there.


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[mcarvey]

Larry,
There are obviously many ways to do things- the command I think you are looking for is sketch filet. I was able to get to get sketch filet to work on arcs without any problem- you need to make sure that any overlapping lines are trimmed off so you have just a corner. To get the radius to line up with the circles, you first need to get out of sketch filet mode, and then either drag the sketch filet radius point to the centerpoint of the circle or select both and then merge points.

Hope this helps,
-Matt

[Larry Dickman]

Larry,
There are obviously many ways to do things- the command I think you are looking for is sketch filet. I was able to get to get sketch filet to work on arcs without any problem- you need to make sure that any overlapping lines are trimmed off so you have just a corner. To get the radius to line up with the circles, you first need to get out of sketch filet mode, and then either drag the sketch filet radius point to the centerpoint of the circle or select both and then merge points.

Hope this helps,
-Matt

The problem arises when the 2 acrs don't intersect. Sketch fillet does not work. (or a line and an arc that don't intersect)

BTW, I saw a Catia guy the other day and had him try it. Catia does it with 1 mouse click, no problem.

SW is the only program that won't do it

[mcarvey]

Oh sorry- I forgot that your arc's don't intersect! Sketch filet won't work- probably constructing circles, making them tangent, and trimming is your best bet. Also, for some things I find that it's often easier to use two features, each with a simple sketch, than just one feature that uses a more complicated sketch. Oh, and keyboard shortcuts are your friend- Alt-A is tangent, and I make "t" trim.

-Matt

[cygnus x-1]

Here's something interesting I just discovered. Sketch fillet will work with non-intersecting entities provided they can be extended to intersect. If not, then no go. This does seem kinda lame since you can make a circle tangent to non-intersecting circles. Why not an arc?

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