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Snap lines for Circular object

Snap lines for Circular object

For a shaft which has a radial pattern in face i want to mention the angle for all the Holes in the Drawing. I used manual dimensioning but thing is that i can't arrange all the dimensions in a circle, which consumes lot of time. Is there any easy way to do so let me know regards Mohan Kumar T
7 REPLIES 7

RE: Snap lines for Circular object

You have to model it like that in the part. I presume you mean like a flange face with a circular hole pattern? So you create your flange and the create a radial Datum Plane (at an angle so you can change it later on) on the face which will be used to drive your pattern feature. Create a cut protrusion on this face (your first hole), create a PCD reference circle as your first feature and turn it into a Construction Circle by RMB clicking. Set your Sketch References as the Datum Plate you created and the centre Axis of the flange. Sketch the Hole you want at the intersection of the Datum Plane and the PCD Reference Circle. Exit Sketcher and cut the Hole. Select the Hole and Pattern it using Axis type, also select the Datum Plane if you want to. Create the Pattern with as many Holes as you like. Create your Drawing and the View you want and go to View, Show/Erase. Select Axis type and Show All, you should have the PCD Reference Circle Axis and the Radial Axis through each Hole. Select Keep All. Unselect the Axis type and select the Dim type, Show All, et voila you have your dimensions correctly shown with angular dimensions and PCD dimension. There might be a shorter way but this is how I do it. Hope it helps. regards Paul

RE: Snap lines for Circular object

That method works, but is a long way. Depending on if you're using just an extrude or the hole tool, the method changes slightly. With the hole tool, place your hole on the face of the flange, pick your first reference as the center axis you're going to pattern around. Under hole placement tab, pick either radial or diameter, depending on whether you want a radius shown or a diameter shown on your print. For your second reference, pick a datum plane that goes thru the axis. This will become your angular dimension. You should now be able to set your radius/diameter and your angle for the holes position. Accept your hole. You can then create a dimension pattern using the angular dimension on the hole. For extrudes, its slightly simpler. Start your extrude tool and create the sketch on the sufrace of your part. Pick the axis and a datum thru the axis as your references. Create a construction line through the center axis and at a set angle of your datum plane reference. Create a circle at the diameter/radius you want your hole to be at, and right-click->construction. Sketch your hole at the intersection of your construction circle and your construction line. Accept the feature. Now you can dimension pattern according to the angle of your construction line you created in the sketch. The downside to doing it this way is that you'll have to sketch a draft circle in your drawing and a group it to its sketch view, or create a separate sketch in part mode to make your circle visible on the print.

Re: Snap lines for Circular object

"Mohan Kumar Thangaraj" wrote:

For a shaft which has a radial pattern in face i want to mention the angle for all the Holes in the Drawing. I used manual dimensioning but thing is that i can't arrange all the dimensions in a circle, which consumes lot of time. Is there any easy way to do so let me know regards Mohan Kumar T

Re: Snap lines for Circular object

I know in wildfire 4, you can select 2 dimensions and right click-align them. You can do this with angular dimensions as well, and also align angular dimensions with linear ones if they share a leader.

Re: Snap lines for Circular object

Mohan, have you thought about the hole table.. where in you will have all the required info for the holes in the x y co-ordinates.Even the manufacturing guys will be happy to see the x y co-ordinates. Pro/e doesnot have radial snap lines to suit your requirements... Need to work around..

Circular Arrangement

Mohan, This won't cause exact "snapping" but can help you get very close visually as you are placing your dimensions. In the Part sketch a Datum Curve on the face of the shaft, picking all of the hole axes as references. Now sketch a Circle at the diameter where you want the dimensions to appear in the drawing; then sketch radial lines from the center of the part through each axis out to the circle; the result will look like a wagon wheel or an empty pie chart. In the drawing you can quickly pick these radial lines for dimensioning and visually place the dimensions on the circle; you can get very close to snapping this way. Hide the Datum Curve in the Part and Drawing when you are done. David

RE: Circular Arrangement

OK, maybe I was assuming it was a hard question! If you assume that you already have the Holes and you want to align all the angular dimensions in the same radial position then it is VERY simple. Simply move the 1st dimension to where you want it and then multi select all the other angular dimensions and right mouse button (RMB), select "Align dimensions" and they will all align with your 1st dimension. regards Paul
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