need help with a sketch

[Anonymous]

hi everyone,i am sorry if this is the wrong place to ask for this.I have to re-create the file impl_fin.stl but without the hole in the middle,i think that i have done the base semi-decently in part2.ipt but i am having trouble with understanding how to create the four corners of the model(i think that they were made with removing material but not sure).can someone give me some tips on how to do them or if possible share a picture of which planes i have to do or sketches,i will be very thankful.i am using inventor pro 2015 and don't know the dimension because i wasn't told.thanks if you can help and i am sorry if i am bothering you.

[JDMather]

First thing you should do is install the Service Packs and Updates for 2015.

2. Do you have precision measuring calipers?

3. Do you have the actual part that you can hold in your hand or is the stl file the only thing that you have?

4. Can you post or link to similar real world part so that the context of use is understood?

5. How much training/experience do you have?  

6. Why are there no dimensions on your sketch?  If I add some of the missing dimensions, they appear to be perfect?  What happened to the missing dimensions?

7. Why are there many missing Tangent constraints?

To my eye, this sketch does not resemble the original geometry?

8. Are you willing to follow instructions as they are presented?

I would have expected your sketch to look more like this....

[Anonymous]

1.ok i will install them.

2.in the program?or irl?

3.the stl file is the only thing that i have.my teacher on sent that so that i can make it without the hole in the middle and test it out with a lattice structure in Autodesk Within.

4.it's supposed to be a medical implant.unfortunately i wasn't able to find pics of it.

5.i have been using the program for a week now since i needed the analyzis function of it,otherwise i have a 2 year experience with solid works.

6.i think that i either deleted them by accident or forgot to add them 😞  (i can be very stupid sometimes).

7.no idea.

8.yes i am willing to follow instructions as they are presented.

[JDMather]

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@Anonymous wrote:

3.  ...my teacher on sent that so that i can make it without the hole in the

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Can you ask your teacher to join this discussion?

[Anonymous]

unfortunately he can't.and wow that's very good.did you use a combination of circles,lines and fillets?that's what i am trying out but as you can see it's not going well.

[JDMather]

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@Anonymous wrote:

5. …. i have a 2 year experience with solid works.

8.yes i am willing to follow instructions as they are presented.

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There is no difference between sketching in SolidWorks and sketching in Inventor.

Surely you must have been given additional instructions by your teacher?

How do you know whether the units are inches or mm or cm?

I can start supplying step-by-step instructions, but it would be useful to know this basic information.

[Anonymous]

it's in mm,that's all i know.

[JDMather]

Step 1.  Start a new mm part file.

Step 2. Navigate to the Manage tab and select Import and select your stl file.

Step 3. Start a new sketch on the XZ plane and sketch the horizontal line as shown.  (don't worry about getting exact to center of circles - we will worry about that later.

Save  your new file and Attach it here for next set of instructions.

Step 1 & 2

Step 3

[Anonymous]

thanks for helping me.

[JDMather]

Step 4. Sketch a circle at both ends of the line.

Step 5. Add an Equal (=) Constraint (Relation in SolidWorks) between the two circles.

Step 6. Dimension one of the two circles as 7mm.

Step 7. Dimension the length of the line as 17.5mm.

Step 8. By eye, drag the sketch geometry such that it is approximately lined up with the imported geometry.

Save and Attach the file here for next set of steps.

[Anonymous]

the below circles will follow the same pattern right?

[JDMather]

Zoom way in on one of the circles to fill up your screen.

You can do better on the manual alignment of your sketch.

[JDMather]

Once you have improved the alignment - add a Fixed Constraint to the midpoint of the horizontal line as shown.

The sketch should change to a darker color.

[JDMather]

Add a horizontal lines approximately to the visual centers of the two bottom holes as shown.

Dimension the line as 30.45mm.

Add a circle at both ends of the new horizontal line.

Add Equal (=) constraints between the two new circles and the 7mm circle above.

Dimension the vertical distance as 18.34 as shown.

Zoom in and line up by eye same as we did the top circles.

LAST of all - add a vertical line between the midpoint of the top horizontal line and the MIDPOINT of the bottom horizontal line.

Attach your file here for next steps.

[Anonymous]

thanks again.

[JDMather]

Turn on your sound...

[Anonymous]

sorry for the delay.was visiting my grandparents at the village yesterday and didn't have any acces to the PC.

[JDMather]

Add the two lines shown at 92°and Tangent to the circles.

BE CAREFUL to NOT select the midpoint of the vertical line when creating these angled lines.

The connection point should be above the midpoint as shown in image.

You do not need to create that Point that I labeled - I just wanted to emphasize to NOT select the midpoint of the vertical line.

[JDMather]

...add a 12mm Fillet between the two angled lines.   Change the Fillet radius to 11mm.

[JDMather]

Add two angles line to the right as shown with dimension of 81.6° and Tangent to the circles.

BE CAREFUL that there are no perpendicular or parallel or colinear constraints added to the two lines.

They will still be underconstrained until the next step.

Attach your file here for the next step.

Edit:  Change the 12mm Fillet radius to 11mm.

See how easy it is to edit a fully defined parametric sketch!