[Ironworks]

Hello,

I'm new to this, and am getting what I think is an excessive amount of a cut where the piece was pierced. See the pic. Any suggestions would be appreciated. The pic is of the top side.

[jemmyell]

You should never pierce right on the profile. Use a circular leadin / leadout pair to take the pierce 'divot' away from the shape profile.

-James

[Ironworks]

Can you explain 'circular leadin / leadout pair'? The PlasmaCAM software does the leadin automatically...

[jemmyell]

The circular leadin is an arc (quadrant arc usually) that starts outside of the profile. The pierce is done at the start of the arc, then the torch makes a semi circle to where the profile starts. The shape you are showing was not cut with a leadin. If it was then the kerf width settings are way wrong to produce gouge like that.

-James

[plasmapunk]

The problem you are having happens to me every once and a while. Without knowing all of your settings. I can give you a few ideas.

First the part you you are showing looks pretty small. So depending on your cut speed there is alot of fast motion going on. Plasmacam seems to have an issue changing direction quickly. There are settings like corner acceleration to help with that issue. Slowing your cut speed will help.

Second and most important, your pierce location sucks. I have attached a file that shows a few pierce location ideas to keep your problem from happening at all. The one in the middle would be the preferred pierce location to get a arrow that you can hold (like the one in your pic). The one on the right would be if you wanted to cut an arrow into a sheet. Finally the one on the left would be an example of a pierce point on a part that has no sharp corners. I added a small triangle to the top to give it a place for a pierce point. After it was cut i would simply sand off the the added material.

C, I have tried the spiral lead in. I have not gotten good results whenever I try it. The start stop point always looks crappy. Besides it's a pain to draw it every time I want to try it.

G

[Ironworks]

Thanks for the pointers and for the file. I'm so new at PlasmaCAM software that I didn't realize that you can specify the pierce point. I'm still not quite understanding how to do it. It seems that the software has a mind of its own when I try to put the pierce where you show it. Your lead-in lines are nice and straight, and mine are now lined up well with the part. Can you help?

Thanks,

- Bill

[plasmapunk]

The pierce point will appear wherever you click on the part. If you click a line with the cross hairs of your cursor outside the part it will put the pierce point on the outside of the part and the opposite will happen if you are on the inside of the part.

To get the pierce point to appear on a corner inside or outside. Put you cross hairs near the corner when you click. If it isn't exactly where you want it undo and try again.

The mind of its own you are speaking of is most likely the auto cut path that plasmacam does if you click on the outer most lines of a drawing that has multiple cut paths on an interior of a part. To stop this, convert the innermost detail of the part and work your way out to the outside line. This way you can specify where you want the pierce points.

I attached a file showing the difference. The part on the left was converted to cut path by only clicking on the large circle around the items within. Plasmacam put the pierce points on the five details inside the circle. The part on the right I converted the details inside one at a time and put the pierce points where I wanted them, then I converted the circle around all of them.

To get the pierce point leadin's nice and straight like I have them. After you convert the detail press E (edit) and grab the end of the pierce point line and drag it where ever you want it.

[Ironworks]

Your explanations were great, and thanks for taking the time to create the sample file -- it cleared it all up.

Now if I could just figure out why, when I import a DXF file from CorelDraw, it sharp corners all have a triangle at the intersections, I'd be all set...

- Bill

[plasmapunk]

Can you attach the file you are speaking of? I will take a look at it.

[Ironworks]

Ok, this DXF file has that issue on the corners. It has criss-crossed corners when I do an Import, Link, then Convert to Cut Path. Zoom in on the corners, and see what I mean. It then takes forever on a complex part to trim all that out.

[plasmapunk]

That is not really a Corel, DXF problem. It will happen even on parts you draw in Plasmacam.

Picture a triangle, take one side and move it toward the center. Now take the other side and move it toward the center. Neither line got shorter when you did that. So you end up with a X at the end where they intersect. Plasmacam connects the two lines with with a short line to keep it one cut path.

You have five options (that I can think of)

1. Convert it and trim all the corners, time consuming but if you are going to cut it out many times it will be worth your time.

2. Change your offset distance to 0. The down side is the part won't be the exact size you may have intended it to be. But on artsy stuff it really doesn't matter. This is the fastest and most used option.

3. Scale the size of the part up really big, then convert it. Downside is the pierce length and gap at end of loop will change when you scale it back down to the correct size.

4. When you draw something radius the corners. The line will offset and the radius will get smaller or even disappear.

5. Don't worry about it. Chances are unless the cross in the corner is huge, you probably won't even notice it. Remember its plasma not Laser.

[Ironworks]

Holy cow!! Do you have any idea how much time you have saved me? Just tonight, I learned more about the software than I did spending hours with the PlasmaCAM manual.

Many thanks. I owe you one!

Regards,

- Bill

[plasmapunk]

Yes I know exactly how much time I saved you. I went thru the same problems when I was learning how to use the program.

A major complaint of mine is how Plasmacam uses the offset feature when drawing in Plasmacam (not the same as when you convert to cut path). In Autocad when you offset a line, the line you offset doesn't disappear like it does in Plasmacam. When you have a closed item in Autocad, and offset the line it does make the line shorter. (That same triangle you drew in Plasmacam would be a smaller triangle in Autocad without the crosses at the end.)

Plasmacam should ask if you want the original line deleted. I use the offset feature when drawing a part all the time. I do very little drawing in Plasmacam, I use Autocad 99.9% of the time and import a DXF file.