Spoon and pickup v shape

[shift1313]

You can extrude with a taper which I what I would do if machining so you know what bit to use. You probably got a zero thickness error. It means that the cut leaves a little alivver or something. Its hard to say without seeing it.

[endlasuresh]

I am attaching the current file just need to cut from the top sketch to down sketch ith slope. you can see the first image which i posted.

http://s000.tinyupload.com/index.php?file_id=07548010129432312442

 

 

I want to cut the light sketch from top to bottom sketch with some slope. I tried loft method, but it needs some distance between these two sketches.

[shift1313]

Suresh, i got your file open and first note for you. Cut-Extrude6 is producing bad geometry. There is no way you are going to machine that.If you are trying to cut away that little sliver made by one of your other cuts use the "Split" tool. You can select the 4 inside faces as the trim tools then split the body.

 

Note 2, sketch 18 is under defined. make sure you have Tangency between your Arc and lins. Also you have a close profile and then 2 extra lines. If you are trying to make a Loft-Cut make sure you make a nice profile with no extra data. You can convert a few lines to construction if you need them in there as reference. Blue lines = under defined.

 

Note 3, your arc of sketch 18 went under geometry so if you tried to use it as a loft cut profile it would leave some solid geometry there.

 

Note 4, a loft cut between these shapes is less than ideal. When you do something like this(loft, boundary etc) you want to make sure that each profile has the same number of sketch entities if possible. if not your shape will be compromised in nearly every case. Because the "base" of your loft cut would have two arcs and a straight line, but the top(sketch 18 ) has just an arc, the loft between these gets messy. If you use a Boundary Cut instead of a Loft Cut you have control over the little green dot that lines up each profile. In a loft it has to be at the start/end of a segment. Because your sketch will end up leaving another small sliver i opted to make a boundary surface so i could extend it. Then i used the operation "Cut With Surface" to remove. You could also draw a profile on the end of your part and sweep Sketch 18 and the base as a path.

 

As it is this thing is going to be slightly painful to machine. The outside at the small end are perpendicular but closer to the top of your image are 82.xx degrees. So this can't be easily done with a normal End Mill or a tapered bit. I would suggest picking a taper on the outside to match a bit you have if that geometry is important to you. Also the cut i just did will require a lot of parallel passes with a ball end mill to cut so make sure you match the fillet at the bottom to whatever tool you are going to use(preferably a little larger).

[endlasuresh]

Hi thanks again, really looks very beautiful.

Yes there were so many mistakes in that file, I tried to cut the part through all Extrude cut1, but it left a 0.03 mm of it, can you specify why it wasn't allowing me to cut whole. Yes the geometry gone bad, but was looking to finish it.

 

I want this to be cut in the extrude cut1, tried even by zooming the area to see if there are any free space.

 

I will check other things too.

[shift1313]

From the beginning suresh make sure that your sketches are fully defined. This means all relations and dimensions to make sure they don't move. Your very first sketch that everything is based on has no dimensions or relations to keep it in place. You should make the lower line have a midpoint relations with the origin. Add angles to the sides and a total height. You can right click on a line and select its midpoint. Make sure the upper lines midpoint is vertical with the origin to keep it all symmetric. The lines were exact lengths so im guessing you used the Additional Parameters section in the line properties. This doesn't add any dimensions to the line and is really not a good way to do things because they do remain undefined.

 

With sketch 2 it was fully defined so that is good! You can simplify things on the lower line by adding a midpoint relation with the origin rather than two 15mm dimensions to keep it centered.

 

Cut-Extrude1. This sketch was under defined again. You have some small 4mm lines that don't need to be there. The reason this cut leaves a bit is because the face you are sketching on is not normal to the end of your part. So you are extruding down but if you look at the sketch "Normal To" you can see. The attached image show this. You need to extend your sketch at least to the lower line of the area you want to cut out or completely past the body. Or you can use other tools like "Split" or cut with surface or something.

 

Cut-Extrude5, this sketch(sketch6) is fully defined but needs to terminate at a different point. What i would do is either make these surfaces and extend them to use the Cut with Surface tool, or make a 1mm offset plane from the bottom(where you are extruding to) and then find out where it intersects your geometry.

 

I feel like you have a lot of angles on the part that aren't needed for the design since you are CNCing the part. With molded plastic parts it is very important to have certain geometry for strength. Keeping a consistent wall thickness and getting strong parts with the tools you have to design with makes it a challenge. With CNC you aren't constrained to the same design criteria. If you are trying to reverse engineer something thats fine but there is no need to have tapered walls/draft on a part like this you are going to mill. i would make it easier on yourself.

[endlasuresh]

Thanks a lot,

I was gone through your steps as per the sketch1, I have made the sketch through dimension, but removed the half lines and made a single line at this stage they were not defined. Thanks for it and I never knew the right click for mid point and there were a lot of tools in the right click.

 

I found the sketch is not touching the boundary line in extrudecut1 of backside and in the last corrected through the back.

 

Some of the sktches Ive corrected and their are lot of angels as per the sample and they designed perfectly.

I am not hoping that I would get the correct shape in cnc which I am currently drawing, because they are no experienced people to do exact things

I don't know about Taper will check in Google to find out and how you cut the part? I mean the second cut? I tried using Split method to cut the part, but it didn't helped in proceeding.

[endlasuresh]

Can you tell me how did you cut this part that is silver sketch. I am in the final to send it in process.

[shift1313]

Suresh I said how to in note4 on my reply with that picture. Did you fix all the sketches and things I mentioned? Figure out anything else about how you will and can cit this?

[endlasuresh]

Hi

Thanks out I have corrected the file and adjusted it in order to finish the drawing. I am attaching the new file and changed a bit from the past file.

http://s000.tinyupload.com/index.php?file_id=68920512893186752867

 

The last thing is making a cavity in plates, can you let me know how to use punch in plates. There were two plates and on one plate the surface of spoon 1mm and v shape of 2mm, half of the middle part comes. while the remaining comes on other plate.

 

Is their any method to make the mold plate cavity as we wish.

I may think sketches may defined or undefined, but just want to finish this part.

[endlasuresh]

I am still awaiting for u

[shift1313]

suresh there are many ways to make cavities but i thought you were machining this part???

 

In solidworks there are different ways to cut away something. You can make a copy of a body then use Combine(which you can use the subtract option). You can use Indent(which is non-destructive meaning the tool body doesn't get removed). Then there is a cavity tool. There are also mold tools which end up using a surface offset and surface cut. All of my videos on this topic are unfortunately locked on VARs websites but here is one i found that a reseller did.

 

[endlasuresh]

No, It is cavity for molding. I watched few of videos in the past for making cavity, but it goes wrong somewhere with me.I tried some of the tutorials, but failed as this is the first time to make a cavity. I was looking to make first insert the piece within plates and then a cavity.

The last one was finished water spike, but the guy few mistakes.

Edited April 23, 2016 by endlasuresh

[shift1313]

can you be more descriptive about what went wrong?

[endlasuresh]

I was following this tutorial, but at mates it is not working also the part 2 unable to keep in straight condition according to the plates.

http://learnsolidworks.com/solidworks_tutorials/how-to-draw-a-coke-bottle-mold-in-solidworks

The mates shows wrong symbol, thats means I did wrong selection. Also these two (mold block and component ) aren't in straight.

[shift1313]

Suresh, i don't see a need to make an Assembly, this can all be done in the part environment. I am sorry i am very busy and just can't walk through the whole process on your part but here is a basic list of things you need to have/do.

 

Your part needs to have split faces breaking up the faces of the solid part where you want the split of your mold to be(core/cavity). This is your "parting line". Ideally this would be a plane or planar face to make things easy. if its not you will have more work to do to make your core and cavity.

 

Next(if doing the process manually and not using Mold Tools) you will need to make an offset surface(zero offset) of the Core and Cavity(2 separate offset surfaces). Depending on your geometry and where these fall you might also need to extend edges using Ruled Surface and/or fill holes in your part. You can then use these surface to do a "Cut with surface" to remove the material from the solid core and cavity of your mold. There is a lot more to it but those are the basics that the SW Mold tools do.

[endlasuresh]

I had given this drawing to in CNC shop and the person tried it to do core and cavity, but they say the drawing is fault. I am attaching the files what they did it.

http://s000.tinyupload.com/index.php?file_id=08663915703251182388

 

http://s000.tinyupload.com/index.php?file_id=38686791147758783789

[endlasuresh]

i haven't finished the last diagram even though I paid to the designer, but he neglected to do.

Can you tell me how to do some cuts using extrude cut feature or some other method.

 

1 The first square in blue should cut with one end 6mm deep and the other end should be 2mm.

 

2 the square which is in slope ( white color)of the plate should cut 2 mm deep.

 

 

[shift1313]

Suresh for the extrude that has to go to an angle one method is to use "up to surface" boundary condition in an extrude cut.

 

First on the side or a plane that would slice the model you want to draw a line that has the appropriate end location. Then make an extruded surface. When you do an extrude cut change the "blind" end condition to "up to surface" and select the extruded surface.

 

On the other cut I dont know what you want it to look like. What needs to change from a simple extrude cut?

[endlasuresh]

I have did finally by using mold time first time,

 

Sorry, I was busy in the last three days with this one so unable to reply. I was asking the seond point was cutting a square or a sketch on a crossed plate. I tried using extrude method but it didnt made.

[shift1313]

Glad you were able to get it working!

 

I am sorry but I still dont understand the other extrude cut. If you know what/where the cut goes to you can always start there. You can loft cut. You can also build it with surfaces to cut the solid if a basic extrude cut wont work.

 

If you can draw on paper or something else how the cut should look maybe I can help more.